# 3D Tutorial (Solidworks)



## JorgensenSteam (Apr 3, 2011)

I am heck-bend on learning 3D modeling, and having a rough time with it.

I made a little headway last night with some 3D modeling concepts, and I will post the ideas I came up with in dealing with 3D here.

After several false starts, I was able to make the frame for the TB5 engine in two parts, and assemble them.

The frame is actually one piece, but I could not figure out how to do a one-piece design.

Here is what I came up with.

Pat J


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## walnotr (Apr 3, 2011)

You are on the right track but you need to think more 3D. You should start by drawing the "L" shape and extrude it to the length you want. Then create additional sketches on the on the planes of the two legs of the "L" to cut extrude the additional shapes in the legs. That way you you get a solid object that doesn't have to be an assembly. SolidWorks is a very powerful program with many features you may never use but can be useful to create many intricate shapes. Keep in mind there are always many ways to attack a problem and jumping in and trying things is the best way to build your skill set. I found it helpful to build 3D models from existing 2D drawings then make the assemblies from the resulting models. Good Luck!

Steve C.


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## coopertje (Apr 3, 2011)

Hi Pat,

In my little experiance with 3D I always attack the parts as if I was behind my milling machine. I start with a solid block and start to cut away material, add radius, drill holes etc. Solid works follows this way of thinking quite well. Maybe not the fastest way to draw a part but for me at least a way that I understand....

Regards Jeroen


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## imagineering (Apr 3, 2011)

coopertje  said:
			
		

> Hi Pat,
> 
> In my little experiance with 3D I always attack the parts as if I was behind my milling machine. I start with a solid block and start to cut away material, add radius, drill holes etc.
> Regards Jeroen



I work the same way with Inventor 2011. This method also helps visualising Workflow when it comes to Milling Time.

Murray.


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## Maryak (Apr 3, 2011)

BoS,

It took me a very long time to get a basic understanding of 3D. Having got this far.............. I start with a plan view of the part and extrude the Z axis into the page. In turbocad the views of the part then follow the 3rd angle projections of said part which is now a solid. From this I take the appropriate view create an outline followed by an extrusion, (again into the page), of the unwanted section then 3D subtract it from the base solid.

Hope this helps

Best Regards
Bob


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## JorgensenSteam (Apr 3, 2011)

Here is an item I found at Dessault.
This helps with the visualization.

Thanks all for the feedback.

I will try the frame again, and extrude as an "L" shape into one piece.

Pat J


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## JorgensenSteam (Apr 4, 2011)

Here is my second attempt at the TB5 frame, this time with an extruded one-piece "L" section.

This works better.

I think I have finally made some headway on the 3D front.
You really do have to think "milling machine", and think in 3D shapes as mentioned by Steve C and Jeroen above.

And I agree with Bob, it has taken me a long time to get my head wrapped around the 3D concepts. If it were not for the fact that so many others seem to use it with ease, I would never attempt it. It is one of those "if they can do it, so can I", but it sure has not been easy to get started.

Pat J


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## gbritnell (Apr 5, 2011)

Hi Pat,
I took an apprenticeship as a metal pattenmaker many years ago. From there I went onto the 'board' as a pattern and corebox designer. All the drawing (2D) was done by hand but you had to be able to visualize the shape of a part to make sectional views. 
When the company got into 3D cad modeling I had gone back to the shop to run machines. It wasn't until we purchased some CNC mills that I had the opportunity to go back to the design and draw part of the trade. They needed 2 cutterpath/CAD modelers so with my previous background I got the job. 
In the 15 years that I worked with the various versions and had to help train upcoming apprentices the first thing I stressed was don't get frustrated, learn it a bit at a time. Some of the versions can be very complex with drop down menus and multitudes of strange looking icons. If a person has only worked with 2D and has never done any type of modeling before it can seem insurmountable.
Having to learn it buy yourself with no mentoring can be a daunting task but certainly not impossible. Just bite off a little at a time and before long it will fall into place. 
gbritnell


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## JorgensenSteam (Apr 5, 2011)

Thanks for the encouragement George.
Solidworks has some extremely powerful features, but is just different enough to throw me. I am starting to make progress though.

Here is the sequence I used for the above part. Although this is a simple part, the difficult thing was coming up with this sequence. Once you figure out the approach, then making model is easy.

For this part, I drew two lines at 90 degrees on the front sketch plane, then offset them by 0.5", and finished the sketch by closing the ends to create the "L" shape.

I then went to 3D mode (the jumping between 2D sketch mode and 3D mode is a confusing thing since you never have to consider such things in 2D), and extruded the angle to 5.75" long.

At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.

Then I discovered how to select a face on the part and rotate it normal so that I can sketch on it in sketch mode.

Other parts of the puzzle were solved when I found the "centerline" in the pulldown toolbar, and was able to use those as construction lines to lay out the work, similar to what one does with layout dye on a real part. I found the "snaps" toolbar, and that was a big help.

Part of the problem with the 3D programs is that they have so many toolbars and tool buttons it is not funny, and some work in 2D, and others work only in 3D, so you have to think in terms of two sets of toolbars, and remember which apply to what.

The constraints thing was throwing me for a loop also, and I must say me and constraints are not friends right now, but I am beginning to understand the importance and power of using constraints, but still learning those. Luckily, the constraints can be deleted if they get too pesky, and I figured out how to do that, but will have to be careful not to work against myself by deleting too many constraints.

Then I figured out you can change the color of an entire object, or just a single face of an object. That can be helpful when you are spinning the part around in 3D space, and need separate colors to keep track of which face you are on.

Another challenge is the fact that any sketch used to extrude into 3D has to be a fully closed figure. I generally draw cleanly enough for this not to be a problem, but the program does not tolerate any figure that is not closed with respect to extruding.

The "cut" feature was confusing, and I assumed (incorrectly) that any sketch used for cutting must also be a closed figure, but that is not the case as I accidentally and happily discovered. I forgot to include one of the 0.5" corner radius in part of the frame (you can see this in one of the screen shots, but luckiliy, I was able to use the "undo" feature to go back one step to the sketch I did for the side of the frame, and add that radius, and then run the "cut" command again.

The cut command can be used to bring a cut "through all" surfaces, or "up to a plane", or several other options which I am still learning.
You can also I think extrude or cut from the center of a plane equally in both directions, which I intend to use for cylinders to great advantage.

So while I have only made a simple part, I have made a quantum leap in getting a feel for what it is that I am trying to do with 3D.
Hopefully this will help some others with this conceptualization.

I have a handle on how to create 2D drawings from the model. In Solidworks, you just drag and drop the model into the basic 2D views, like front, side, top, isometric, etc. That is simple, but I am still figuring out how to get the dimensions to display properly in the 2D drawings.

My ultimate goal is to create an animated moving with a translucent cylinder so that I can see the engine running and look for interference problems.

Beyond that, I want to link in an Excel spreadsheet so that I can enter values in the spreadsheet and have the model change size accordingly.

Thanks again for the feedback. I think I am on a roll now with 3D.

Pat J


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## JorgensenSteam (Apr 5, 2011)

Here is more of my second attempt at the frame.


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## JorgensenSteam (Apr 5, 2011)

Here is more of my second attempt at the frame.


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## JorgensenSteam (Apr 5, 2011)

Here is more of my second attempt at the frame.


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## walnotr (Apr 5, 2011)

BigOnSteam  said:
			
		

> At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.



It is a good idea to try and fully define drawings as you go. It can make life simpler when and if you go back and modify the drawings. If a drawing is not fully defined, strange things can happen when you change an angle or dimension. It can be very frustrating at times and not always necessary, but as a rule you should work in that direction. Defining a drawing is not only accomplished by dimensions but also by "properties". i.e. vertical, horizontal, concentric, coincident, co-linear, and the like. Many of the properties are automatically selected for you as you create a drawing but are not always desirable. You may not want the center of an arc coincident to a line for example. All of these things can easily be changed once you find your way around and learn what works well for you when making your drawings. It is very helpful to look at drawings made by others to see how the have tackled a problem.

Steve C.


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## imagineering (Apr 5, 2011)

You might find it helpful, (I'm assuming it works in Solidworks), to extrude to both sides of the Origin Plane.
ie; instead of a 100mm Extrusion being Z0 to +Z100, the Extrusion exists as -Z50 to +Z50.
This forces the Origin Plane to be in the Centre of your Extrusion, which is very helpful when laying out Sketches later on, as you now have a Centre Reference to work from/to.

Murray
(Inventor 2011 user).


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## JorgensenSteam (Apr 5, 2011)

Thanks Steve and Murray, I will try those ideas.

Pat J


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## Donrecardo (Apr 6, 2011)

> At first I was getting a lot of error messages about the model not being fully defined, but I figured out how to turn that off. I will have to come back later and figure that part out.
> 
> 
> 
> ...


[/quote]

If you want it fully defined just go to the menus at the top and choose Tools/Dimensions/Fully define .  It will pop up a window where you click on all entities in sketch and then click calculate, it will then fully define it for you.

As for looking into the engine to look for interference problems , rather than make it translucent , click on the section button and slice it on any plane , you will see all you want then

Don


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## JorgensenSteam (Apr 9, 2011)

Thanks Don-

I will give those ideas a try.

Here is a quick drawing I made tonight for the frame.
2D drawings in Solidworks are created by opening a part file, and dragging and dropping on the 2D layout sheet. Each time you drag to a new position, you get a different view.

I guess this is where the power of 3D modeling begins to kick in.
It only took seconds to create this sheet, and any future changes I make to the model with be automatically updated in every view on every 2D sheet that I have created, and all the dimensions will also update automatically.

Now all I have to do is figure out how to get the dimensions on the 2D sheet.

Pat J


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## Lockstocknbarrel (Mar 13, 2012)

Hi Pat 
I had a play as well...................
Just love Solidworks went to Night School to learn.
If you want the file let me know.
What version are you running.
Kindest Regards
Beagles


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## lee9966 (Mar 13, 2012)

One thing I learned with SW is not to put too much in a single Sketch. Lots of sketches each determining a single feature makes it easier to work with for me. 

For example if you have a surface that needs holes for mounting and holes for something else it is tempting to put all the holes into a single sketch. What I would do instead is to make one sketch for mounting holes, another sketch for the other holes.

Hope that helps, I am self taught an maybe others will correct me.

Lee


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## JorgensenSteam (Mar 26, 2012)

_I am going to revisit this post since I understand 3D modeling much better now than I did a year ago. These steps are generic, ie: they apply to pretty much any 3D program including Alibre.
This post was added on 3-26-12._

Lee has an excellent point, if you keep your sketches simple, then it is much easier to come back and correct a part of the design that may have a problem.

My approach to learning 3D was to purchase Alibre (I have Alibre and Solidworks), and just start the program and use it, since I have used 2D drawing programs for years.

So my problem was I would start Alibre, and then try and use it like a 2D drawing program. Big mistake, Alibre cannot be used in the same manner as a 2D drawing program, at least not if you plan on making 3D models.

A typical CAD 2D program has only one mode of operation, ie: you start the program and then draw on the screen using the mouse. What you see is what you get, and you can draw anything anywhere with impunity.

A 3D modeling program has two modes of operation, and you cannot do anything unless you understand what the two modes are, and when to use what mode. The two modes of a 3D program are "sketch" mode, and "modeling" mode (I think those are the correct terms).

Sketch mode is 2D drawing program, but you cannot use sketch mode exactly like you would use a 2D drawing program, I will explain why shortly.

Another big problem with 3D modeling is that you cannot use it without thinking about what you are going to do with it first. It would be like trying to machine an intricate part in the milling machine, and you put your part into the vise, start your mill, lower the bit into the work, and just hope something good happens. I can assure you nothing good will happen! You have to plan what you want to do first, such as define datum plane, define cuts, define the bits you want to use, shape of cuts, hole locations, fillets, etc.

So initially, I would open Alibre, try to draw something without a real concept of 3D, and then fail miserably. I did this for months.

So how do you get around the initial program shock?

My recommendation for an approach to 3D modeling is to start by visualizing the finished part that you are trying to model. Next, take that part, and slice it once like an orange, and look at the outline of the cut or section that is created. For an orange, a sectional view will look like a circle. So for 3D, you have to draw a circle, or for a sphere, actually a half-circe. You draw the half-circle in "sketch" mode on a 2D plane, and then revolve that sketch into a 3D sphere.

As you get into more complex shapes, it gets more confusing, and so you have to visualize breaking a part down into its basic geometric shapes. For example, a steam engine cylinder has the main cylinder containing the bore, the flanges on the ends of the cylinder, the steam chest, steam chest flange, valve face, ports and passages, counterbore, cylinder head holes, etc. 

Start by figuring out what the single-most basic and fundamental shape of the part is. For a steam engine cylinder, that would be a cylindrical tube. So focus on creating a cylindrical tube first, and then adding additional features onto that tube.

You can make a 3D tube by just drawing a circle "in sketch mode", and extruding that shape into a solid tube at the length you want.


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## JorgensenSteam (Mar 26, 2012)

A little more discussion of "sketch" and "model" modes is in order, along with a discussion of the "planes".

3D programs typically start by displaying three basic planes, the "front, right and top" planes (see photo below). In order to get an idea of why you have these planes, think in terms of placing a piece of raw metal in the milling machine. You have to know which surface or plane you want facing up towards the bit. Same with 3D.

If you look at the button I circled on the upper left, labeled "Sketch", you can see that the button is depressed. What does this ALL IMPORTANT button mean? Took me a long time to figure that one out, with lots of hair pulling. The sketch button is analogous to lowering the milling machine bit onto a particular plane just before you start cutting. When you are in "sketch" mode, you have basically lowered the bit to the correct plane, and are ready to start cutting. If you jump out of "sketch" mode, you have raised the bit up, and are not on any particular cutting plane.

How do you use the "sketch" button?
First, make sure the button is not depressed (you are not on any plane).
Then you can select the sketch button, and then pick the plane you want to begin with, or reverse that and pick a plane first, then pick the "sketch" button. If you don't pay attention to the position of the sketch button, then you will be cutting a lot of air.

How do I draw the basic starting shape of a cylinder, such as a rod shape?
I visualize my cylinder on a table top, with the top of the table being the "Top Plane". If I slice my cylinder like slicing a hotdog, then I see a circle in section, and that circle will appear in the "Right Plane".
So to create a cylinder, I first I select the right plane. Make sure the "sketch" button is not depressed. If the "sketch" button is depressed, then un-depress it, and then select the right plane, and pick the sketch button again (you are putting your cutting bit on the right plane, perpendicular to the surface of the right plane when you pick the sketch button and pick the right plane.

Draw a circle on the right plane as you would using any 2D CAD program.
Go to the features toolbar, and select "Extrude", and extrude the circle into a cylinder, see below.


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## JorgensenSteam (Mar 26, 2012)

When you select a sketch plane, generally (but not all programs) will rotate the plane you select "normal" to you, so that you are looking down perpendicular on the plane.

This is akin to you leveling your milling table and getting it perpendicular to the bit.

You can change the view of the plane at any time by rotating the model (with Alibre I think by holding down both mouse buttons and dragging), but if you are in the process of actively working on a given plane, and accidentally rotate the plane, it is the same as rotating your mill table while you are milling (disaster).

If you inadvertently rotate your plane while you are sketching on it, find the buttom that returns the plane normal to your view, and then continue your sketch.

Below are the same three planes as above, but with the right plane rotated normal to the screen. The top and front planes appear as lines, since you are viewing these planes on edge.


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## JorgensenSteam (Mar 26, 2012)

Draw a circle on the right plane. The size of the circle is not important since you can select the circle and edit the size of it at any time.

Edit the size of the circle to the dimensions you want, or approximate dimensions you think you will need. I will use a 1" radius for this circle.

From the features toolbar, select EXTRUDE, and extrude the circle out from the plane, as shown below. I like to extrude from midplane, out in both directions, but you can extrude from the right plane out in one direction only, or extrude from the midplane out in both directions.

You can come back and adjust the length of the extrusion at any time, so just pick some random approximate length, in this case 4".

Note that your initial sketch shows up as the blue circle (color may vary in Alibre). This sketch generally does not show up once you have extruded, otherwise there would be too many sketches in view. You can always come back to this or any other sketch and modify the size, shape or position of it later.


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## JorgensenSteam (Mar 26, 2012)

What do I do next?

Well first, retract your bit away from the right plane (using the milling machine analogy) by pressing the "sketch" button to unselect the sketch plane mode (note, solidworks automatically unselects the sketch plane after every 3D command, Alibre may also).

Your 3D model should look like that below.
I have rotated the model (hold down both mouse buttons and drag in Alibre) to view it orthogonally, and note that the "sketch" button is not depressed, and I am not on any particular plane at this point, just looking at the model from out in space.

Notice that on the left of the screen, the program is maintaining a list of 3D FEATURES I have created, and the SKETCHES used to create each feature.

It should be noted that if you want to change a sketch, you can return to this list and select the appropriate SKETCH name from the list, to edit the size, shape or position of a sketch.

If you want to change the length of an extrusion or a cut, you must select the name of the FEATURE from the list, in this case "Boss-Extrude1", and edit that.

Pick the sketch name to edit 2D sketches, pick the feature name to edit 3D features. In Solidworks, I can pick a name, right click, and edit. Not sure about Alibre.

A common mistake is to pick an existing sketch, edit it, and then forget to jump out of sketch mode to get back to a 3D view.

You must remember at all times whether you are on a sketch plane, or out in space looking at the 3D view. Same thing with a milling machine. Do you have the bit against the work, or have you retracted it? Its a critical thing to keep up with at all times.


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## JorgensenSteam (Mar 26, 2012)

Next you decide to bore a hole in the rod for the cylinder bore.

I have two choices, I can add a separate CUT feature to cut the bore, or I can go back and edit the initial sketch of the circle.

As mentioned above, there is much to be said for isolating most of your steps into one feature completed at a time. The features are called the PARAMETERS of the 3D model, and thus the term PARAMETRIC MODELING. The beauty of 3D modeling is that any parameter can be changed at any time, and you can relate parameters to each other, so changing one parameter automatically changes others (use this feature carefully).

Occasionally, you may want to combine two features into one sketch, and we will do that in this case.

If I wanted to keep the bore a separate feature, just select the right plane, go into sketch mode, draw the circle for the bore diameter, extrude a cut from midplane, and get out of sketch mode.

In this case, I pick "SKETCH2" from the menu on the left, go into sketch edit mode, and then add the bore circle to the first circle I drew. When I exit sketch mode by pressing the sketch button, the model automatically updates to show the bore, as indicated below.


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## JorgensenSteam (Mar 26, 2012)

So lets add the flanges.

Make sure the SKETCH button (circled in red) is not depressed (make sure you are not in sketch mode).

Pick the end surface of the cylinder as shown below.


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## JorgensenSteam (Mar 26, 2012)

Click the sketch mode button to create a new sketch which will be on the same plane as the end of the cylinder that you just selected.

Rotate the sketch plane that you just created normal to the screen, to look like below.


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## JorgensenSteam (Mar 26, 2012)

Draw two circles, one which matches the outside diameter of your cylinder, and one that is the diameter of the outside of the flange.

You are creating a new feature by drawing a new and uniquely named sketch, and then extruding that sketch into a flange.


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## JorgensenSteam (Mar 26, 2012)

Extrude the sketch that you just drew (two circles) into a flange, and make sure the extrusion is towards the center of the cylinder, not away from the center of the cylinder.


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## JorgensenSteam (Mar 26, 2012)

Generally you only have to draw half of an given shape like a flange, since you can mirror the feature to create the flange on the other side.

In the example below, we make sure we are NOT in sketch mode, select the 3D mirror command, pick the mirror plane (in this case the Right Plane), then pick the flange. It is very easy to pick the wrong plane and/or feature to mirror, make sure you load each dialog box one at a time, and get the right data in each part of the dialog box. If the command did not work as you intended, use the undo button and try it again, and pay closer attention.

It sometimes is tricky to make sure you picked only the feature you want to mirror, and not some other feature.

Don't confuse mirroring 3D features (done when not in sketch mode) with mirroring 2D lines (done in sketch mode). Same feature, but one mirrors lines, and one mirrors 3D solid shapes.

Also, don't confuse 2D sketch commands with 3D feature commands, they are not interchangeable. Use the 2D sketch toolbar only when you are in SKETCH mode, and use the other 3D toolbars only when you are NOT in SKETCH mode. 

Again, it is super critical to remember at all times which mode you are in and what you are trying to do while in that mode. They need a warning tone and a light to remind you sometimes "Hey, you are trying to use a 3D command in 2D sketch mode", or vice versa. This is the single biggest problem of using 3D modeling in my opinion, you cannot ignore mode for a second.


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## JorgensenSteam (Mar 26, 2012)

And now, since the flanges were added with respect to the ends of the cylinder, and extruded inwards, then I can stretch the 3D cylinder (modify the length of the cylinder), and the flanges will automatically follow, but still maintain the same flange dimensions.


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## JorgensenSteam (Mar 26, 2012)

Lets say you don't like the outside diameter of the flanges.

Which part of the model defines the outside diameter of the flanges?

Answer: Sketch5, shown in the menu on the right.

So edit sketch5 (go to sketch mode, but go to "sketch5" by editing it from the list on the left of the screen, not by pushing the sketch button), select the outer circle, re-size it to the diameter you want, and then exit sketch mode.

Presto, you have a larger flange, as shown below.

And note that since you mirrored the flange, the mirrored flange automatically changes its size at the same time (smarter not harder is my philosophy).

Steps shown below are:
1. Select the SKETCH5 sketch from the menu on the left (I think you right click and then pick edit in Alibre, that is how you do it in Solidworks).

2. Your model now displays SKETCH5 (shown with blue lines).


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## JorgensenSteam (Mar 26, 2012)

3. Rotate SKETCH% normal to the screen.

4. Edit the outside circle to the new diameter.

5. Exit sketch mode.

6. Rotate the model so you can see it in isometric form.


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## JorgensenSteam (Mar 26, 2012)

Want to put holes in the flanges.

Pick sketch mode, pick the outside face of the flange, draw one hole where you want it in the flange, array that hole around the flange for the total number of holes you want, extrude-cut the holes.

Then mirror the holes you just created to the other flange.


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## JorgensenSteam (Mar 26, 2012)

I never got around to finishing the explaination of why you can't use the 2D drawing portion of Alibre exactly like the 2D drawing portion of any 2D CAD program, since they do exactly the same thing.

For 3D modeling, you are drawing a sketch on a plane, and then either extruding a solid, or extruding a cut into 3D space (generally).

In order for the 3D modeling program to define the limits of the 3D surfaces you are creating, the sketch from which this 3D surface is derived has to be a continuous and closed shape.

So when you are in sketch mode, and drawing a 2D sketch in preparation for a 3D extrusion, remember, you can use any 2D command you want (copy, move, rotate, mirror, offset, trim, line, circle, ellipse, etc), and draw any number of lines, circles, reference lines, etc., but when you get your sketching done, you have to clean up all the miscellaneous lines and things so that you are left with a continuous outline of some shape.

For instance, you cannot draw a circle, and then draw a line across that circle, since the 3D program cannot figure out two halves of one circle.

All lines have to be snapped to endpoints of other lines or shapes.
If you don't snap all of your lines, you are left with tiny gaps between the ends of the lines, and you can't see the gaps, but the program can.

This was a big stumbling block for me as far as learning 3D.
I pay very close attention to drawing complete sketches which enclose a single outline of a shape (remember, outline only, no lines in the middle, or anywhere else).


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## JorgensenSteam (Mar 26, 2012)

Another idea that I had a hard time wrapping my hear around is the question of how the program treats the 3D solids that I was extruding from my sketches.

I was baffled to no end, since I could draw a shape, and then cut a slice out of the center, and have two pieces remaining, but the program treated the two pieces as one object.

Remember that once you extrude a shape, no matter how you modify that shape later, the program remembers that the base shape (in our example the tubular part of the cylinder) is still defined as one piece.

Solidworks (and maybe Alibre) has an option to either "merge" or "not merge" things like the flanges that I added to the cylinder. I almost always merge any additions to the initial base object.

On rare occasions I do not allow the program to merge things, but be aware, if you do NOT merge the objects, then any changes in a base dimension will not automatically move the added parts such as flanges.
So I generally always merge any changes to the base part.

As I add features to the base 3D part, although the features may be merged into the base part, they are still separate entities, and are listed as such in the data column on the left side of the screen, and therefore, I can edit and change any single feature without necessarily affecting any other feature.

If I add a feature, such as our cylinder flanges, and add them with respect to the end planes of the base feature, then modifying the base feature can also result in modifications to things created with respect to that feature.

Play around with that and you will see what I mean.


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## JorgensenSteam (Mar 26, 2012)

And.....(sorry, this is a bit long-winded)........


One of the great secrets of successful 3D modeling is to draw your more complex sketches in a 2D program such as AutoCad, and then import them into your 3D program, and extrude them.

I am much more familiar with drawing complex 2D shapes in AutoCad than I am in Solidworks or Alibre, so this allows me to leverage my large knowledge base in 2D AutoCad for use to create sketches for my 3D program.

For simple shapes, I just sketch things in Solidworks or Alibre directly.
Alibre has an IMPORT command for importing dwg sketches from other 2D CADD programs. Solidworks allows you to open a DWG file directly in Solidworks, but both programs do the same thing (import 2D sketches from other programs).


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## Marinesteam (Mar 26, 2012)

I started reading this thread with interest as I'm a long time user of Solidworks and was curious as to how a new user would approach Solidworks.

May be I can offer a few tips that may help...

You will find that there is no need to use another 2d program to do the sketching before importing into Solidworks. Solidworks can leverage data from already existing 2d data, but if you are creating new geometry in another program you will only be wasting your time. I understand that it may be easier now as you already understand the other software but in the long run it's best to let go of how it's done in 2d and just jump into the 3d mindset.

In Solidworks, like many 3d packages, there are many ways to skin the proverbial cat. Many ways will work and one is not necessarily better than another. The most important thing is to determine design intent and model to preserve this as much as possible. In many cases this means NOT to model the part like it would be machined but model in a way that leverages the existing geometry and the parametric features of SW.

Use your "heads up display" to your advantage. SW will give you many tips while modeling and sketching. One of the most powerful is inferencing and pointer display. While sketching, your mouse pointer will change depending on where your pointer is in relation to geometry on the screen. For example: if you enter a sketch and select the line tool then mouse over the origin, the pointer will show a set of concentric circles. This means that if you click, the beginning of the line will have a relation added making it coincident to the origin. If you then pull the mouse, the line will stretch from the first point to the pointer, if you move the elastic line so that it is nearly vertical the inferencing line will appear. Clicking now will draw the line and add a vertical relationship to the added line. These relations are the power of Solidworks and allow the drawings of geometry with the addition of very few dimensions.


I could go on but the best thing you can do is to go through the SW tutorials (in the help menu) from Getting Started and work your way along. Do a few, then apply what you've learned to some of you own parts then do a few more. You'll be up to speed in no time.

Ken


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## JorgensenSteam (Mar 26, 2012)

In summary, using 2D CAD, you create separate sketches for the front, top, side, etc. for each individual engine part. These sketches are not dynamically linked, and the sketches do not have to be complete or correct in any way. You plot/print collections of sketches on drawings, as shown in the first example below.

When using 3D modeling (2nd example below), you create a sketch for each part, extrude that sketch into a 3D solid, and generally modify that solid with additional features of bosses, cuts, etc.

Using the "Bottom-Up" approach, which I prefer over the "Top-Down" approach, I make one model and save one model file for each part.

I then create an assembly, which begins as a blank model.
I insert one part into the assembly at a time, and align the parts together with "mates" as I go.

Once an assembly has been completed, it can be run in simulation mode, so that operation of an engine or valve gear can be seen visually while it operates.
The program can flag any interferences in red.
You can also check alignment of holes in mating parts, etc.

It is important to remember that an assembly is a file separate from each part file, and if I change the model for any part, the assembly automatically reflects that change.

If the assembly and simulation looks good, then I create a drawing for each part file.
The drawings are exactly what would be printed or plotted from a 2D CAD program.
Again, keep in mind that each drawing file created is a separate entity from a part file or an assembly file, and any changes to any part by modifying its 3D model are automatically reflected in every assembly, drawing, exploded view, bill of material, motion study, etc.

And remember that you can assemble a few parts into Assembly No.1, and then a few different parts into Assembly No.2, and then create another Assembly No.3 that contains one or more Assemblies No.1 and 2 (something to keep in mind, not always used, but sometimes useful).


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## JorgensenSteam (Mar 26, 2012)

_Ken posted:

"In many cases this means NOT to model the part like it would be machined but model in a way that leverages the existing geometry and the parametric features of SW."_

I could not agree with this more.
In the beginning, I modeled exactly like one would machine a part, but quickly found out that if you reverse the order of things sometimes and in some instances, and do things slightly differently than machining, you can build 3D models much more efficiently, and edit them much more efficiently too.

_and another Ken quote:

"I understand that it may be easier now as you already understand the other software but in the long run it's best to let go of how it's done in 2d and just jump into the 3d mindset."_

I agree with this to some extent, but not entirely.
Some sketching commands are much better in Solidworks, and some are much better in AutoCad. Unfortunately, I find the grips in Solidworks to be very lacking. Somewhat making up for the poor grips in Solidworks is the ability to hover adjacent to a point, and automatically have a horizontal or vertical line drawn to a point, when you are in alignment with that point.
If I could have all of the power of AutoCad 2D in Solidworks sketching, then yes, I would dump AutoCad.

For very complex sketching, I would always use AutoCad, just becaue creating the same sketch in Solidworks would take me forever.
Most people don't do very complex sketching, but I do.

I also use AutoCad 2D for initial geometry layout, and rough out the basics of the design in section first. You just really cannot do that sort of "scratch pad" preliminary rough and incomplete design in Solidworks very easily, in my opinion, and I am sure I can't, I tried, and I understand Solidworks very well now.

_Ken posts:

"Use your "heads up display" to your advantage"._

I would add to this, learn these items and don't ignore them as I did for a long time. These items are critical when you are creating sketches. Little pictures pop up next to the mouse cursor depending on where you are, and tell you all sorts of critical information.

If I could take one single thing from AutoCad and add to Solidworks, it would be the excellent grips, grip sizes, and grip colors that you can use in AutoCad, and the superb clarity of how these grips are displayed in AutoCad. Solidworks just doesn't have it in this area.
The focus in Solidworks is on 3D features, but they come up far short of AutoCad in the 2D area (my opinion only, others will not agree with this).


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## Maryak (Mar 26, 2012)

I approached this conundrum in a slightly different manner.

In TurboCAD the 3rd axis is the one going into the page. So if you extrude, loft or draw a primitive it comes out of the page at you, (positive), or into the page away from you, (negative). and its' zero point is on the current workplane.

Hope this helps.

Best Regards
Bob


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## JorgensenSteam (Mar 26, 2012)

Bob-

I am sure everyone has their favorite approach.

As Ken mentioned, there are many ways to do any given operation, and many different ways work well, for different reasons and objectives.

As my wife will tell you, I moaned and complained to no end for months about learning 3D modeling. I made very serious attempts to master 3D a number of times, and each time gave up in total dispair and frustration, certain that I would never learn 3D.

Rick and many others on HMEM kept saying "I am not finding it that difficult". Gosh, that was all I could say (or something to that effect).

Then I woud have partial sucess here, and a little success there, but still lots of problems. Then it started to click, and then, a year later, bingo.

I started learning 3D about a year ago, with no prior knowledge of it.
My intelligence level is somewhere between a Neanderthal and an amoeba, proabably more towards the amoeba if I had to guess.

So the following is a collection of one year of trying to learn 3D. 
I post this not to brag on myself, but to show you the progress that can be made in one year starting from scratch to creating pretty good models.

Here are the first crude models I made.


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## JorgensenSteam (Mar 26, 2012)

And then a few more complex models.


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## JorgensenSteam (Mar 26, 2012)

Confidence started to build, as did complexity.


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## JorgensenSteam (Mar 26, 2012)

Every sucess built upon previous successes until things got pretty advanced.


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## JorgensenSteam (Mar 26, 2012)

And finally some recent models.


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## JorgensenSteam (Mar 26, 2012)

The sky is the limit with 3D modeling folks.

Don't say you can't learn it, it can be done I assure you, but not over night.

Model them, assemble them, and run them, all on the screen.

If you want to get dirty, then build a real one in your shop.

Rick was right, it is not that hard.

Edit: I think I am going to change my screen name to "AmoebaMan".
I like the ring of that. (You have to have read the previous posts to get this).


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## JorgensenSteam (Mar 27, 2012)

Stanley 20 hp steam engine valve and cylinder.


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## JorgensenSteam (Mar 27, 2012)

Stanley valve and seat assembly, shown in "wireframe" mode, with hidden lines visible.

This mode is useful when you need to see the lines that are behind your current sketch plane. You can use the lines in the background to draw new shapes from. Solidworks allows you to directly transfer a copy of hidden background lines to the current sketch plan (very nice feature).


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## Marinesteam (Mar 27, 2012)

UNIcastings  said:
			
		

> _Ken posted:
> 
> 
> I agree with this to some extent, but not entirely.
> ...


_

I don't know what tools you are looking for in sketching but I find that SW is a very powerful and fast sketching tool. I think that you may be getting hung up on grips and how it is done in 2d. I personally, never draw with the grid as I find it annoying, but I know those that do. Sketching in 3d is different than in 2d. Relations are the KEY to modeling in solidworks and also the biggest switch from 2d sketching. If you get your mind wrapped around this concept, all else will easily follow. 

The order of sketching is important, Draw your geometry in a rough form then add the relations (or let these get added as you draw) the finally add the dimensions. Before adding the dimensions, exercise the sketch to test the relations. Add only the dims needed to fully define the sketch. Exercising means to pull some of the sketch points around to see if the sketch relations behave as they should. ie: Vert lines stay vertical, equals are equal, etc. Remember to use the geometry previously defined by the model (if any) to define as much as the sketch as the design intent allows. 

I have used Autocad since V10. I still use 2d Autocad (actually the equivalent Draftsight) for panel layouts as the mfg files for components come in dxf form. I don't find the sketching tools in Autocad to be more powerful, I just find them to be more appropriate for the type of drawing done in 2d.



			
				UNIcastings  said:
			
		


Ken posted:

I also use AutoCad 2D for initial geometry layout, and rough out the basics of the design in section first. You just really cannot do that sort of "scratch pad" preliminary rough and incomplete design in Solidworks very easily, in my opinion, and I am sure I can't, I tried, and I understand Solidworks very well now.



Click to expand...




I do scratch pad models all of the time. The sketching is fast and sketches in a .swprt don't even need to be made in 3d. I often do quick sketches instead of trig. It's nice to have the visual confirmation of the math (use the driven dimension to check the solution)

The nice thing about the parametric (relations) is that you can sketch the design intent and then quickly test other sizes or configurations just by changing a few dims. 

It helps to keep individual features simple to allow these changes with less effect on the rest of the model or causing the model to "explode". If you have modeled with design intent in mind the important features will remain as needed while you experiment with the remaining geometry.

This is an animation of the engine that I am currently in the process of building. I have been drawing some of the parts as I go along to check the prints for accuracy before making chips. The model is incomplete but there is enough to check the motion in the animation.

[ame]http://youtu.be/R0YFwrQH58A[/ame]

Cheers_


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## rhitee93 (Mar 27, 2012)

I was a power AutoCAD user, and had a real hard time making the switch to SolidWorks. The first time I tried to switch, nothing made sense and I gave up. The second time I tried to switch over, it didn't go much better.

The third time, something just clicked, and I have never looked back. It is fortunate because I have to use it a lot at work, but I truly do enjoy using it more that AutoCAD.

It took me a while to understand mates in assemblies. Here is a shot of a Kouhoupt engine I drew up just to play with mating features. Some day I need to finish it, but each component is mated so that if you turn the crank, the components all move correctly.


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## JorgensenSteam (Mar 27, 2012)

Ken-

That is a great looking compound.
What sort of bore and stroke are you using on that?
I like it a lot.

If you compare AutoCad 2D with Draftsight and the 2D sketch part of Solidworks, the basics are the same, but there are a number of commands that are present in AutoCad that are not in the other programs.

If you happen to use or need to use these commands frequently, then it becomes very tedious and time consuming not to have them.

One example is the Divide command in Acad. I use it constantly designing engines. Don't see it in other programs.

I also have customized Acad, since I have used it for production for many years, and any time saved is money saved. A well customized Acad setup is many orders of magnitude faster than a plain 2D program.
I also integrate Excel with a lot of Visual basic programming into Acad.
Can't do that with the others I don't think.

So for me, going from Acad to another 2D program is like getting out of my modern automobile and driving a model T. Yes, both cars go down the road, but not the same way or at the same speed.

I don't use grids. I do use grips extensively.
It would be nice to be able to toogle ortho lock on and off in Solidworks.
That is one feature I really use and miss.
The way that Solidworks handles ortho is much more combersome to me most of the time, but not always.

I can rough out a basic layout of an engine in Acad in minutes, and nothing has to be a closed shape, etc., just rough sketching. Not so with other 2D programs (for me).

I agree about relations, and I need to work on those.
At this point, the relations get in my way when rough skteching, and I keep getting unwanted relations as I am rough sketching.

Can I turn off relations? and then once the sketch is done, add back just the ones I want?

Relations is one of the big reasons I can do rough sketches much faster in Acad. You don't need relations to make a rough layout, they just get in the way.

You can do a whole lot of customizing Acad in many ways, and I use scripts, diesel, visual basic, etc. to customize Acad. I have been extremely frustrated at not being able to customize the 2D part of Solidworks and Draftsight.

Brian-

It took me a while to figure out mates.
I almost have them figures out, but keep finding new tricks.

The simulations are invaluable for checking to see if the engine will run correctly.

Turning the surfaces of the cylinder transparent is also invaluable as far as being able to see what is going on while the engine is running, and also from a design standpoint visually.

I have started using Solidworks at work, and you can save a lot of time by using the relationships. It is great for laying out complex equipment, when it is critical that things all fit together exactly.


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## Admiral_dk (Mar 27, 2012)

> One example is the Divide command in Acad. I use it constantly designing engines. Don't see it in other programs.



I hope that I'm not stating the obvious, but I can't help thinking that you should see it the other way around, because there's a multiply command i 3D. Do a feature (hole etc.) and multiply it in a linear or circular way x number of times.


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## JorgensenSteam (Mar 27, 2012)

I use the divide command in Acad when I define the two end holes, such as the outer two holes in a steam chest cover, and then want X number of equal spaces between them.

I can locate one hole, mirror it, use the divide command, and then spot the holes between, all in seconds, and all without using a calculator.

For an array command, you have to know the spacing before hand, so you have to stop and use a calculator.


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## Marinesteam (Mar 27, 2012)

UNIcastings  said:
			
		

> That is a great looking compound.
> What sort of bore and stroke are you using on that?
> I like it a lot.



It's the York compound from Elliott Bay. Dims are HP 3in, LP 5.25in and stroke 3.75in. 




			
				UNIcastings  said:
			
		

> If you compare AutoCad 2D with Draftsight and the 2D sketch part of Solidworks, the basics are the same, but there are a number of commands that are present in AutoCad that are not in the other programs.
> 
> If you happen to use or need to use these commands frequently, then it becomes very tedious and time consuming not to have them.
> 
> One example is the Divide command in Acad. I use it constantly designing engines. Don't see it in other programs.



My point was that many of these commands simply aren't needed in SW sketches or have better ways of accomplishing the task. Many of the reasons that you might divide a line in a sketch simply don't exist because the sketch can be related to other existing geometry. Divide may be a good example. The quick way is to draw a line segment then use the split entity tool to split it into connected segments, then add an equal relation to each segment. But there are probably several other ways to accomplish the design intent more efficiently. Using formulas may be one way but I'm not sure what you want to accomplish.



			
				UNIcastings  said:
			
		

> I also have customized Acad, since I have used it for production for many years, and any time saved is money saved. A well customized Acad setup is many orders of magnitude faster than a plain 2D program.
> I also integrate Excel with a lot of Visual basic programming into Acad.
> Can't do that with the others I don't think.



I used to be a big LISP proponent. I find that SW is pretty good on it's own and there isn't much automation that I need to do that would make the customization worth it's while. I use SW every day for huge projects. SW does have the availability of Macros and VB API programming. Excel can be used to drive configurations, which are really handy, but that would be a thread all on it's own.



			
				UNIcastings  said:
			
		

> So for me, going from Acad to another 2D program is like getting out of my modern automobile and driving a model T. Yes, both cars go down the road, but not the same way or at the same speed.
> 
> I don't use grids. I do use grips extensively.
> It would be nice to be able to toggle ortho lock on and off in Solidworks.
> ...



You can turn off the automatic creations of relations but I'm not really sure why you would want to Right click the open area of a sketch and look for relation options). Relations are created by how you direct the cursor. Ortho mode is simply not needed because of how SW sketches. Draw a line by clicking the first point in the line tool then drag the mouse a distance either horizontally or vertically from the first point. Watch the cursor, You will see the relation icon appear next to the cursor arrow when the cursor is near horizontal or vertical from the original point. If you click the line will have the relation added to it automatically. If you don't want the relation move the mouse until the cursor changes to just the arrow and the relation won't be added. You have full control of how relations are added just by moving the mouse to the proper location using the heads up display. It's way faster than having to change modes while sketching. 

I'd argue that you do want relations while drawing rough sketches. As this is what keeps the sketch "under control" while it's being created and is how the design intent is built into the part. How one gets into trouble is by putting too much geometry into a single sketch. Simplify sketches and separate features and you will go a long way toward harnessing the power without getting burned by relations. Makes for much more robust parametric models.

One of the big leaps of logic that I needed to make when changing from 2d to 3d is that the 3d sketches are rubber bands and not unrelated entities like in 2d autocad. Sketch with this in mind. Draw your rough shape letting the relations be added automatically where appropriate. Pull points around, see if the sketch behaves the way you want. Add or edit relations as needed to reflect the design intent. Finally, add as few dimensions as needed to fully constrain the sketch. It's really nice being able to pull stuff around where the related parts stay in proper relationship to each other and where the parts that have no relation can be manipulated to see other possibilities. I don't know if this quite makes sense in words, it sounds way more complex than it actually is.

Cheers

Ken


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## petertha (Mar 27, 2012)

UNIcastings  said:
			
		

> I use the divide command in Acad when I define the two end holes, such as the outer two holes in a steam chest cover, and then want X number of equal spaces between them.



Im self taught but why not consider the power of SW equations in this example? You have the defined physical dimension between two end holes, call it X. Then make the interspacing spacing dimension a dependant equation = X /(number of desired spaces). And that can be patterned. Now with SW parametrics, if X ever changes to a new dimension, the inter-distances scales in/out automatically. In non-parametric programs (assume autocad?) you would start at the beginning again, erase the original line, draw a new line, re-make the divisions etc.


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## Marinesteam (Mar 27, 2012)

UNIcastings  said:
			
		

> I use the divide command in Acad when I define the two end holes, such as the outer two holes in a steam chest cover, and then want X number of equal spaces between them.
> 
> I can locate one hole, mirror it, use the divide command, and then spot the holes between, all in seconds, and all without using a calculator.
> 
> For an array command, you have to know the spacing before hand, so you have to stop and use a calculator.



The parametric nature of either pattern tools (feature or sketch) can be used to your advantage. I tend to use the sketch pattern tool for hole patterns.

The cool thing is that you can define the pattern many different ways each having it's own advantages. Start with an 5 x 1 linear sketch array of a point that is on the origin. Once the array is created drag any of the newly created points around. You can constrain any point to any sketch feature or other geometry (including the other array point) as you see fit. Think of the possibilities. The only problem with SW arrays is if the number of features is changed you will dangle (loose) relations attached to those sketch features that no longer exist.

Cheers

Ken


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## JorgensenSteam (Mar 27, 2012)

Ken, Peter-

I need help with equations and using Excel with Solidworks.

Can you guys give us a tutorial on that?

I have yet to figure all that out.

I think equations are a separate thing from using Excel, but act in a similar fashion, ie: you can relate variable, such as X=1, Y=X*2, etc.

Thus Y depends on the value of X.

But as far as using this stuff, I haven't been able to do that yet.

I am not aware of the "split entity" tool. I will look that up.

As far as using Acad for sketching, I use it generally to arrive at overall proportions between all the parts vertically and horizontally.
I don't need an accurate sketch, or even lines that are snapped to anything. Unlike a sketch in SW for a single part, I use AutoCad to lay out the entire engine, in rough form, as mentioned generally to establish proportion and visual effects. I would not want any relations when doing this, as it is not a part sketch, but a different application/use.


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## Marinesteam (Mar 27, 2012)

UNIcastings  said:
			
		

> I think equations are a separate thing from using Excel, but act in a similar fashion, ie: you can relate variable, such as X=1, Y=X*2, etc.
> 
> Thus Y depends on the value of X.



The excel part is different and it is covered well (much better than I could) in a tutorial in the Productivity Enhancement section titles Design Tables. Design tables are in excel and can do anything that excel can do just be aware of the formating requirements of SW. (All listed in the help files)




			
				UNIcastings  said:
			
		

> As far as using Acad for sketching, I use it generally to arrive at overall proportions between all the parts vertically and horizontally.
> I don't need an accurate sketch, or even lines that are snapped to anything. Unlike a sketch in SW for a single part, I use AutoCad to lay out the entire engine, in rough form, as mentioned generally to establish proportion and visual effects. I would not want any relations when doing this, as it is not a part sketch, but a different application/use.



If you want to make your whole model be truly parametric you really are talking about assembly sketches which is a whole topic of it's own. I tend not to do Top-Down driven designs but the function is available. I do quick test sketches in a .swpart document to test ideas but either way relations are very much a needed part of the process. Example: You want the piston rod to be centered over the crank shaft but the angularity is determined by the crank throw and the con rod length. These parameters are all relations, some geometric and some dimensional. Like the piston rod being vertical to the crank axis. If you think about it this way you can design by locking in the parameters that you know and let the others fall into place. 

Cheers 

Ken


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## petertha (Mar 27, 2012)

UNIcastings  said:
			
		

> I think equations are a separate thing from using Excel


Here is an example using SW dimension equations. They are very powerful. I divided the line by two, just for simplicity. The steps were:
- dimension the base length, a known value
- insert the feature somewhere along the line
- smart dimension the feature just as you normally would
- now select the dropdown (or now = sign in SW-2012)
- 'point' to the reference dimension, incorporate as part of the equation so /2
- it shows a math summation symbol reference to indicate a function vs a 'hard' dimension
- test by altering the base dimension, volia!


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## petertha (Mar 27, 2012)

last pic. Changed the base dimension tosomething different & the feature 'auto-calculated' itself parametrically.

You can similarly incorporate all sorts of math functions.. sin, cos, square-root etc


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## JorgensenSteam (Mar 27, 2012)

Peter-

That is cool.
I did not know that was where you entered the equations.

Looks simple but powerful, I will try it.

Thanks, I appreciate it.


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