Cannot place constrain in Inventor
 

So I have a problem in Inventor. I downloaded the van door motor from FIRST CAD Library. And I made a mounting plate for it with 3 screws for the bolts and one hole in the middle for the shaft to go through. I try constrain the two together in a assembely. I first mate the van door motor to the face of the mounting bracket. Then I mate the centerline of one bolt hole to one of the holes in the bracket. Next I try and mate a second bolt hole to the second hole in the bracket except I get an error. What should I do, should I make the holes in the bracket adaptive or what?

Re: Cannot place constrain in Inventor
 

try an insert constraint. Then u can offset however far you need to get the right fit.

Re: Cannot place constrain in Inventor
 

Try making them adaptive only if you're interested in having a nice looking assembly. Do not use the adaptive part as a template for making a real plate.

The bolt pattern of the van door motor model provided in the virtual kit of parts is incorrect. Unfortunately, I don't know what the correct dimensions are offhand, nor can I measure one.

Re: Cannot place constrain in Inventor
 

I know that when designing parts I shouldn't use adaptive things, this is just a general Inventor question. The plate is already made, I just want to model it. I tried the insert command but it didn't work, the problem is that the distance center to center of the holes is not "EXACTLY" the same (at least I think that's the problem). And I got the van door motor from FIRST CAD Library, not the VKOP.

Re: Cannot place constrain in Inventor
 

Well I found out a way to do it, sort of. First make the holes adaptive. Then constrain them and take away the adaptivity. This is really wierd and I'm surprised it worked. Does anyone know a better/cleaner way to do it?

Re: Cannot place constrain in Inventor
 

Seems like the holes in the motor do not align with the holes in the plate. My recommendation is to start a new assembly. Click Place Component and place the motor. Then click Create Component and click the mating surface on the motor. A new sketch will start after you enter the information in the dialog box. Click Project Geometry and project the holes in the motor to the new sketch for the plate. Continue to build the plate. The holes will line up exactly. A word of caution - if the motor is not accurate as some have written - your plate will match the model but not the real thing. Hope this helps.

Re: Cannot place constrain in Inventor
 

The mounting holes for the Van Door are 1/4" dia on a 1.5" radius. They are 120 degrees apart. I typically have trouble getting it to line up properly. So here's how I handle it.

First use an INSERT constraint on one of the mounting holes on the motor. I usually use the one that sticks out at 90 degrees to the motor axis.

Then I use an angle constraint between the edge of the mounting plate and the web supporting the mounting hole. Adjust the angle as needed to get the holes to match.

The speculation that the problem is not getting the numbers to match is probably correct, but we don't have the ability to specify the numbers to the tolerance needed to eliminate the issue.

Re: Cannot place constrain in Inventor
 

so basically you are trying to place 3 holes on 3 pegs?

Re: Cannot place constrain in Inventor
 

The way by creating a component off of the motor sounds like a good idea. Haven't tried it yet but I will. Thanks.

Re: Cannot place constrain in Inventor
 

Paul,

The reason it is a good idea is because once you have an existing stock component, like a motor - and hopefully an accurate model - you do not need to analyze the component to create a new sketch for a mounting plate. You just project the geometry and let Inventor do the work. It is a much more productive and intuitive method in my opinion. And you won't get that "Can't create a constraint..." thing anymore. Believe me, I have been there. It drove me crazy. If you need more help, just yell!