CAD Tips?

Hi guys. I know very, very little about CAD software, so I was wondering if some of you guys could give me tips.

I pulled some components off of the Vex website and started to try and mate them to make a simple chassis. I find mating is kind of really tricky. Since the holes are bigger than the screws and there’s no easy way in Solidworks to find the center of a hole it was hard to constrain a bolt to them. The bearing blocks looked easier but the little square tabs are just a tad bit off the right size. So, how do you guys mate stuff quickly and easily when they don’t fit perfectly together? Any other tips or tricks I should know about?

I also had many of the same questions, right now I have had to manually move the parts and eye-ball them into the right position, and rotate them by hand, and measure if it is 90 degrees flipped or not, which takes a very long time, that is why I have not built much with Autodesk Inventor. Sorry that I could not help you, but I would like to second the question.

I have the exact same problem with Autodesk Inventor… Any help would be appreciated.


Don’t worry about getting the screws perfect, honestly not needed. THe biggest Vex CAD issue for me has been lining up the square shaft with the certain components. My solution has been to create center points (called datum points) on several objects.


This… not acceptable. In CAD we “mate” objects together as they would be mated in the real world. In order to mate any object you’ll need to create an assembly file.

Once inside an assembly you can drop different parts into the scene. Use different types of mates to snap your parts together. The only time I find myself manually moving parts is when I have to see a certain part that is blocked from view by another part.

I also seriously recommend SolidWorks, Autodesk Inventor is fine but I prefer SW.


How exactly do you drop parts into the scene once you have an assembly open and you have some of the parts downloaded? I can open the parts individually but I can’t seem to drag them anywhere.

Depends on the program, in SolidWorks there is a button in the top left that says something like “insert component” which allows you to bring another SolidWorks part into the scene.

It is important to note that you may have to take a format such as a STEP file and import it, then resave it as a SolidWorks or Inventor part file before you bring it into an assembly.


In Autodesk Inventor Professional 2010, you place parts by clicking on the “Place” button in the Assemble tab. Then you browse to the file that you want to insert, and click “Open.”
To “mate” parts in Autodesk, use the Constrain tool (found under the same tab).

Thanks guys. I’m using Inventor and I’ve managed to merge parts together, although not as lined up as I wanted it to be.

However, I was wondering why all my parts are gray? I’ve seen in some of the renderings around that the parts are colored, such as the green clutches and the black motors. I was thinking it may have something to do with when I’m opening the STEP files and in options, there are things such as “Individual Surface Bodies”, or “Single Composite Features”?

All of the parts start out in gray once you get them from the Vex website, you must color them yourself. To do so, you can click on the “Color Override” drop-down menu, (you will see “Color Override” when you hover your cursor over it) it is located at the top of the screen, near the middle, to the left. From there you can change the color of the whole part, and to change just a single piece of a part, you can right-click on it, click on it, select “Properties” and then, click the drop-down menu, and select the color you want.

So for all my aluminum, bearing blocks, etc. I should go in and add center points and stuff for alignment purposes? This will get annoying, but I guess it’s a one time thing.

What material properties in Solidworks should I set for steel parts? Aluminium parts? Shafts? I assume Delrin is Delrin…

I only bothered to add a few where I needed them.

Whatever looks best if your after visuals, if your looking for simulations, can’t really help you because I don’t know the alloy of the Vex steel.


Main thing I would want to know is weight (calculating drive gearing, etc), but I should be able to estimate density or manually set the weight of any part anyway.

Need the alloys, let me know if you find them…

Sorry about the dumb question, but I’m having trouble setting center points on my Vex CAD files. Specifically, the square filleted holes in Vex metal don’t seem to leave me with many options. Any tips?

I originally discovered that none of the square, rectangular solids and cutouts that VEX designers made have axes in them. If you want to constrain a “square peg to a round hole”, (or a round screw to a square hole, or square shaft to a square hole) you have to create the missing axis, or center points in the solid. A pain, I know. It should have been done when the designers were first creating the solids, but oh well…

I had to go back, take all their parts in Inventor, or .STP format, (I work primmarily in Inventor, but am familiar w/ Pro-E & SolidWorks)

  1. make a sketch on the face perpendicular to the desired axis,

project existing geometry,

Create sketch lines that meet in the center (across corners of a square, from centers of unequal sides, etc.)
to find the geometric center,

then add a point. Add a inscribed circle also (good idea).

Pattern the sketch elements, particularly the points, circle and axis line.

Close the sketch,

start a new sketch at the other end of the proposed axis,

repeat above from (1.)

Then, add an axis along the centerline of the solid that can be used to constrain a cylindrical object (like a screw, which has built in axis) to the artificial axis that you’ve created in your square hole in the sheet metal, nylon bearing block, etc.

If it’s a patterned feature, like the sheet metal plates, c-channel, etc., just find the C to C and pattern the artificial, created axis or point.

Note: after you’ve done constraining your assembly, go back into the individual parts and turn off visibility of the "constraint construction"elements. Axis lines, sketch elements, etc.

Lots of work, but then you’ll easily and accurately be able to constrain round to square, and vice-versa.

Perhaps I haven’t dug into the forums enough for tips, but I was wondering how the premade parts could be cut.

Also, for mating holes, it’s similar to what ngineer suggested, but probably simpler:

  1. Open the part for which you need an axis defined in a hole
  2. Find the desired hole
  3. Define a midplane between two parallel planes on two opposite faces of the square hole.
  4. Repeat Step 3 for the adjacent two faces that are opposite each other.
  5. Define the axis as the intersection of the two midplanes.
  6. Hide midplane visibility.

Check out this post:

Quick search of “Cutting Parts” got me what I wanted very quickly. :wink:


I find that Pro-E is great for making assemblys, which can then be animated using 3Ds Max, Blender, Maya, or whatever other program you want to use.

I work with Inventor at the moment, and haven’t used SolidWorks for a while, so can’t say whether it would work the same but…

What I do is to put in one sketch to find the centre point, level with one of the faces of the metal,

close the sketch and then click on the dropdown next to “Axis” and select “Parallel to Line through Point”, then click on the point and one of the outside edges of the part, meaning you only have to do the one sketch each time…

You can then turn off the visibility of that sketch, as you won’t need it anymore - if you do want a pattern across your whole part you can just pattern the work axis itself

This may be between the different software packages, but in Inventor (2011) there is an option on the “View” tab for object visibility.
This allows you to turn off all the sketches/work axes etc. at once, rather than going through and doing it one by one.

I think it also leaves them still visible in the sub assemblies if you have to go back later and open one of them to do more work…