3D Tutorial (Solidworks)

[Maryak]

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

 

[JorgensenSteam]

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.

 

[JorgensenSteam]

And then a few more complex models.

 

[JorgensenSteam]

Confidence started to build, as did complexity.

 

[JorgensenSteam]

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

 

[JorgensenSteam]

And finally some recent models.

 

[JorgensenSteam]

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).

 

[JorgensenSteam]

Stanley 20 hp steam engine valve and cylinder.

 

[JorgensenSteam]

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).

 

[Marinesteam]

Ken posted:


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 because creating the same sketch in Solidworks would take me forever.
Most people don't do very complex sketching, but I do.

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.

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.

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

 

[rhitee93]

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.

 

[JorgensenSteam]

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.

 

[Admiral_dk]

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.

 

[JorgensenSteam]

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.

 

[Marinesteam]

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.

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.

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.

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.
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 sketching, 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 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

 

[petertha]

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.

 

[Marinesteam]

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

 

[JorgensenSteam]

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.

 

[Marinesteam]

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)

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

 

[petertha]

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!