Part locked in place when one constraint is added

[SCASTILLO-RMI]

Using Inventor 2019. Starting about a week ago I noticed that when applying a constraint I lose all freedom of movement with the part.

For example, I choose a mate constraint to place a small block on a flat plate. Previously once the parts were mated I would still be able to slide the block left/right/up/down along the plate. Now once the constraint is applied the part is locked. It will not move until I add another constraint, or delete the previous one.

This appears to be limited to one assembly but it occurs regardless of which parts I am working with or constraints chosen . I checked and there are no errors, grounded parts or conflicting constraints.

Any help with this one would be greatly appreciated.

[Anonymous]

I've had the exact same problem as you. The majority of the solutions suggests some sort of failure in the constraints, which I found was correct, but the 'design-doctor' was unable to detect it.

I went through all parts and constraints, but no visible flaws, however I provoked a over-constraint situation and afterwards the design-doctor listed no only the over-constraint but also another, not previously shown, constraint-problem. After deleting the troublesome constraint everything went to normal.

I am sure this is a Inventor problem as the malfunction in the constraint situation was not detected.

[johnsonshiue]

Hi! Usually, the behavior is related to pre-existing constraint failures. Or, there could be geometric issues. Another possibility is about LOD. In non-Master LODs, the constraints with unloaded components are solved using the cached geometry. Sometimes Inventor got confused about what geometry to be used.

Activate Master LOD and do rebuild all. Do you see the failed constraints? Does the assembly still lock up?

Many thanks!

[Anonymous]

You are correct, this was a constraint failure, but not one detected within the design-doctor - it has been hidden until a provoked over-constraint. LOD's has been on the scope, but all was set to master, so nothing there.

The model is now functioning as it should.

for info - I went through all parts within the model and looked at all constraints with no failure or flaw in the constraints before it were solved.

[mapsuporte]

Hi Everyone,

I have a customer that is facing the same problem. We resolved it discovering the "sick constrain". 

The icon "Show sick" was gray, but we expand the relationships and find a relationship with a yellow icon. After exclude it, we was able to move/slide the part.

Best Regards,
Vinicius Moreira

[Anonymous]

This happened to me today. While reading thru this thread I could not come up with an exact solution, however it was constraint related. I traced my problem back to a part several parts away in the build up. The problem part was over-constrained with a mate and flush constraint while also having our preferred insert constraints. I deleted the 2 constraints and voila! The assembly moves again!

[mrichard]

One constraint a washer to a pin, now with the mouse you can not move those parts. But they can be moved with another constraint.

 

[mrichard]

To fix this issue I removed the Component Pattern. Not sure why this fixed the issue, look like a bug to me.

 

[johnsonshiue]

Hi! This is a bug in 2023.0. It will be fixed in 2023.0.1 update (available soon).

Many thanks!

[eric.dekeuster]

Helo Will, I hath the same problem as you described, my solution was just making a new Assembly and the constrains are working again. So, maybe the first composition ore assembly was corrupt.

[johnsonshiue]

Hi Eric,

What release are you on? I am not aware of a systematic issue like this. We did have a  regression in 2023 RTM preventing components from moving, when there is a component pattern. This has been fixed on 2023.0.1 and later updates. Please make sure the applicable Inventor updates are installed.

Many thanks!

[anthonyzepeda1969]

I have had the same issue randomly even when starting a completely new assembly with just 3 components. Assign a simple constraint and then none of the parts move freely without using the "FREEMOVE or FREE ROTATE" option.

Go figure.

[johnsonshiue]

Hi! There are multiple reasons which may contribute to the behavior. 1) The part or the subassembly is adaptive. 2) There are Tangent or Transitional constraints. 3) The component was created by Component Pattern. 4) There is a corrupted constraint. 5) The geometry is bad. 6) There is slight deviation in the geometry (non-orthogonal faces).

Please share an example here. Forum experts can help take a look.

Many thanks!

[anthonyzepeda1969]

I'm referring as I stated a new assembly with just a few components (2/3). Zero sub assemblies. Just a basic assembly. The behavior does not occur all the time. It is random.

1.) The part or the subassembly is adaptive. - No sub-assemblies nor adaptive. No adaptive parts.

2) There are Tangent or Transitional constraints.- Nope just mates, face to face or axial.

3) The component was created by Component Pattern. - No component patterns.

4) There is a corrupted constraint. - It happens when there are literally just one constraint. The very first one. lol

5) The geometry is bad. - Normal square or flat surface.

6) There is slight deviation in the geometry (non-orthogonal faces). - Nope we do not work with complex geometry, everything is basically flat or round. 😀

[johnsonshiue]

Hi! If you happen to see a repeatable case, please share it here or send it to me directly johnson.shiue@autodesk.com. I would like to understand the lock-up behavior better.

Many thanks!

[Manuelcamposcosta]

This happens to me quite often I'm pretty sure it's an Inventor problem, because sometimes I just need to ground something around that part and it works, I believe it's because some of them are complex to calculate.

This has happened in Solidworks to me also but much less frequent.

[anthonyzepeda1969]

I actually never had that happen to me in SW. But yeah I think it's a random thing in Inventor.

Well theres not much complex about recatngular parts. lol 

[johnsonshiue]

Hi Folks,

If possible, please share an example that exhibits the behavior. As I have mentioned earlier, there are several ways to lead to a lock-up assembly. Some may be reasonable but most cases should be bugs. Without an example, it is impossible to tell which is which.

One option you may consider turning on. Go to Tools -> App Options -> Assembly -> check "Enable redundant relationship analysis." When this option is enabled, the assembly constraint solver will do a more thorough solve, as opposed to the default quick solve. In some cases, the default behavior, though performant, can lead to incomplete DOF analysis.

Many thanks!

[anthonyzepeda1969]

I understand the need to actually look at a file on your own system. However sharing is not always possible. Also, in my instance when it is literally 3 files with basic recatnagular geometry in a newly created file there are no other constraints to confilict with. Just doesn't seem like worth the time.

But will try to share when possible.

What about remote trouble shooting? Is that an option with Aitodesk? 

[johnsonshiue]

Hi Anthony,

In very rare case, we would debug remotely. It is not a typical process. You mentioned that it happened to a simple dataset. Please share it with me directly johnson.shiue@autodesk.com.

Many thanks!

[anthonyzepeda1969]

I've already moved on with that assembly. 

Next time I have the issue i will share with you.