3D Tutorial (Solidworks)

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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).

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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).

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

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).

 

[Marinesteam]

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

 

[JorgensenSteam]

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).

 

[JorgensenSteam]

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).