I can not get my constraints to work correctly when switching a part in an assembly.

[Anonymous]

I changed one part in an assembly and now I cannot figure out why the constraints are no longer working.  The housing/body used in Rev 6.0 was a solid body.  I need to make a few changes so I re-created the part and replaced the component in the assembly.  I expected to have a few constraint issues but I cannot figure out why I am running into this issue even after following the same sequence.  

I am sure it is something simple that I messed up or am overlooking.  Any suggestions would be greatly appreciated.

I have attached the following:

- A video of the assembly that functions as expected.  SWX3 Rev 6.0

- SWX3 Rev 6.0 - The assembly file and parts.

- SWX3 Rev 7.0 - The assembly file and parts.

Thank you in advance,

Patrick

[JDMather]

The Cable is grounded at the Origin in both assemblies, but WEDGY HOUSING is grounded in a completely different location in R7.

I also see numerous underdefined sketches - this is bound to cause issues.

[Anonymous]

I appreciate your input.  I am aggressively trying to learn Inventor so I am certain the quality of my work does not reflect my determination nor my typical attention to detail.  I just don't know what I don't know yet.  Which are the "undefined sketches" that you are referring to? 

The primary issue is that I cannot constrain the wedges to the path in the housing.  Nothing was constrained to the cable so I cannot imagine that would have any impact (a rookie assumption).  Which attributes could potentially cause the constraints to no longer function?  Could the design of unrelated parts have an impact?

[johnsonshiue · Accepted solution]

Hi! This is a imprecise geometry issue. The constraint fails because the geometry is slightly off. Open SWX3 - WEDGY BODY - PJA.ipt and edit Sketch9. Measure the angle at the top. You will get 10.01 or something. This is wrong. It should be 10 deg precise just like the imported part.

Many thanks!

[Anonymous]

Johnson,

It worked!  I spent nearly 6 hours editing and messing with these parts to get the constraints to work until 3am this morning.  I cannot thank you enough for your help with this.  Such a simple fix for a terribly frustrating problem.  

Thank you,

Patrick

[johnsonshiue]

Hi Patrick,

You are very welcome! This kind of precision issue can be hard to detect. Inventor constraint solver is quite precise (assembly constraint and 3D body up to 0.00001mm; 2D sketch up to 0.000000001mm).

So, when the constraint fails to solve, either the geometry is imprecise or there is conflict somewhere (or a bug).

Like JD said, there is a reason that you want to fully constrain the geometry (logically). In this way, the geometry is guaranteed precise and all the downstream operations will be easier to understand.

Many thanks!

[Anonymous]

Lesson learned and that makes a lot of sense.  I have gone back and created dimensional constraints on these parts and will continue to do that moving forward.  Thank you again.

[BDCollett]

Have a look into Top Down modelling, for something like this if you model it all in the same part and then create your assembly from that it is much easier to avoid issues like you encountered. Modelling parts separately and then assembling them can lead to tiny differences that as you have found out can be very difficult to find.

Another way if the parts you are working from like the wedges are a standard part is derive their details (like that angle) into the Housing part so again the dimensions are exactly the same and reference each other.

The "underdefined" sketches JD was referring to means that you have not constrained them. If you drag them around they will change and move. It's best practice to make sure all sketches are constrained. This was unrelated to your actual issue.