Autodesk Inventor Question

I have made half(one side) of a drive/chassis and i was wondering what the easiest way to repeat it on the other side. I tried copy pasting the whole thing, but that didn’t work. I don’t want to mirror it because it is hard to get the spacing just right. And whenever I try to just place 2 of the same assembly into a new assembly it wont let me use the imates so it is harder to finish off.

Is there an easier way to do it or do i just need to import 2 into a new assembly and use regular constraints?

I have tried to find the best way to do this time and time again, without much luck. iMates don’t appear between assembly layers, unfortunately. However, you can demote a part so that its iMates will appear. If you do need to create a true mirror, with a non-symmetric assembly, here is the method that I use, to keep Inventor from creating all new mirrored versions of the parts:

  1. Create a new part.
  2. Under the “3D Model” tab, in the “Create” portion of the ribbon, click “Derive.”
  3. In the window that pops up, browse for the assembly you want to mirror, and open it.
  4. Under the “Bodies” tab, for “Derive style”, select the third option, “Maintain each solid as a solid body.”
  5. Under the “Options” tab, check “Mirror assembly” and in the drop-down list, select the plane you want to mirror the assembly about. Usually this is the YZ Plane.
  6. Click “OK” and wait for it to finish before saving the part.
  7. Import the derived part (the mirror of the assembly) into your entire robot’s assembly along with the original assembly.


Mirroring takes a lot of time and hard drive space because it has to create each part again. What I did was to create a second model of the drivetrain, move some things around, and rotate it. However, this will only work if it is mostly symmetrical from front to back.

Thanks for the ideas. Anyone have any other ideas?

I will try to mirror it as it appears to be the best option so far.

I gave up even trying to mirror the left and right sections of the drive, it always caused more problems than it solved. I now always build the drive as a single sub-assembly to which the lift and further parts are then added.

If you want to copy a set of constrained parts, don’t use CTRL-C, CTRL-V, use the ‘Copy’ button, as this retains all constraints in the copied parts. After that, right click on constraints that are different on the opposite side and use ‘edit’ to change the positioning of each constraint.

Thanks leonb2273. The copy paste buttons worked. For others reference the buttons are under the tools tab.

Anyone have any idea why I can’t copy and paste in inventor under bootcamp on my macbook? I can do it fine on my windows desktop so i know i am doing it right.

Do you guys make different assemblies for the chassis and lift and other parts and later combine them in a new assembly or do you make it all in one assembly from the start?

Anyone else have any input??

I tried this and the result is the same as when I do CTRL-C and CTRL-V. Any ideas on what I am doing wrong?

I’ve noticed in Autodesk 2014 that the CTRL-C CTRL-V trick does hold constraints. At least for me it did, can’t test for you now though I’m 5000 miles away from my computer.

If you use CTRL-C,V it should work with bootcamp, also you can configure the trackpad to recognize two finger touch on bootcamp as well allowing you to two finger right click.

I find it good practice to make subassemblies. So Naturally I make, a lot of them It saves time, and it allows you to easily have different variations as you iterate your design. Also you’ll find it saves lots of time as well, there are a few “cheats” in CAD with subassemblies when it comes to mirroring and what not. Personally I CAD half the robot, Save that assembly and mirror it as I iterate.

I know how to do it on bootcamp, but nothing happens when it try to do it with more than like 3 parts. Its not a slow or old computer either. It would use my desktop but am not at home for a while. How do you use multiple assemblies? Do you make them totally separately then add one to the other or is there some better way to do it that I don’t know?

The typical method is to make small sub-assemblies, then create a new assembly and piece together the sub-assemblies in that larger assembly. This creates a hierarchy that makes sense and is easy to use and follow.


So do you stay in the same .ima file and start with say one side of the chassis and make it a sub assembly then start on the lift and make it another sub assembly in the same .ima or do you make 2 separate ima’s and put them together?

Typically, I will create one .iam for half of the drive, then close that and create an .ipt for the mirror of it using the Derive feature. I will then close that and create another .iam for half of the lift, close that and create a .ipt for the mirror of it using the Derive feature. Then, I will close that, and create one last .iam for the intake, and finally close that. I will then start a new .iam and place all of the above .iam and .ipt files I have created into it to piece them together, creating a .iam of the entire robot.


Thats exactly what i was looking for! Thanks a bunch Jordan!!!

You are welcome! Glad I could help.