Components won't move or rotate anymore

[rataylor]

Hello, seems as though the bigger my assembly file gets the more I start getting messages that it can't "solve" a constraint. And some of my components are "sick". Is my file too big? Is there a "get well" button somewhere so constraints aren't sick anymore. What to do? I want to do my Ratio constraints on the gears but want to align the teeth before doing so, but they won't turn anymore. Is there a constraint to relax to do that? As usual, I try for hours trying to figure this stuff out before asking for help from the pro's. Thanks again! Later, RT.

[Cadmanto]

@rataylor 

Are you loading the full model or in Express mode?

Another thought is, can you make sub assemblies of some of these parts to work in a smaller more controlled assembly environment?

I see similar responses from Inventor as far as the inability to move or rotate components that are not constrained.

Once I reset Inventor the ability comes back.  Not seeing the sick constraints or components just because my assembly is larger.  If I change something yes I see that, but that is to be expected.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2021

[rataylor]

I'm using student/instructor 2019 download version. I'm must assume all the parts are in the zip. Please elaborate on "full" or "express" mode settings. It's probably important to use "full model" mode at the beginning to make everything work correctly. I would avoid the "Express" mode if I knew how to avoid it because I'm learning this 3-D stuff on my own, no hurry.

     The "reset" command must be in later versions as none of the dropdowns had it nor the right-click menu either. Or is "reset" a generic term for something else? Also, "Level of Detail"(in parenthesis) is now in the name of the assembly. That's a thing that's new to me, but is probably due to clicking a bunch of stuff to get the components to move to no avail. Many thanks!

[JDMather · Accepted solution]

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@rataylor wrote:

 Is my file too big? 

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It is not "too big".  A lot of other issues though.

I didn't dig deep, but I suspect that I would have more sub-assemblies.

I would use a lot of Insert constraints.

I would assemble and properly constrain (including Motion Constraints) more or less as I would in the real world>

(That means I would not have a full assembly and then try to figure out the constraints.)

So - if I were to attempt to fix this - I would open another instance on my second screen and start a new assembly going in very disciplined steps as though it were real parts in front of me.  (One difference from real world though is anything that moves together as though it was one component - I would combine into one sub-assembly - so these for sub-assemblies would be Demoted into one sub-assembly.)

I envision about 9 top level Insert Constraints and the necessary Motion constraints, not much more at the top level assembly.

Going back to the beginning though, I would not have any patterned (or very few) sketches.  All of my patterns would be feature patterns.  Looks like a fun project.

[mcgyvr · Accepted solution]

Mate 39 and 66 have lost one or more of their references.. This typically happens when you change a part and that feature that was used in the constraint is deleted. 

Most of the rest seem to be related to the fact that you have TONS of missing dimensions/under constrained parts..

NEVER leave a sketch until its 100% constrained..

For example.. Bestbearinghousing there is a distance of 0.281684038 in from hole to hole feature..

You are trying to constrain it to Big Gear Back Plate which has a distance of 0.281250000 in from hole to hole..

Inventor will complain as it should when you try to constrain between those 2 features as the distance is not the same..  I'm sure all the rest are issues just like that..

again NEVER leave a sketch until its 100% constrained.. Inventor even shows you in the bottom right corner when active in a sketch how many dimensions are needed and if a sketch is fully constrained.. 

[mcgyvr · Accepted solution]

I also recommend using "Insert" constraint with a face to face hole to hole direct connection where a part is essentially bolted to another like in the constraints discussed above. 

[Cadmanto · Accepted solution]

@rataylor 

To follow up with your response, the attached link will explain what the express mode is.

Didn't realize you were working with the student version.

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/Inve... 

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2021

[rataylor]

Hello, thanks again for your response. BTW, is there some way to "relax" the precision settings to, maybe, disregard inaccuracies of sketches or constraints less than, for example, .001 in.? Just wondering, because dimensioning takes up time when there are so many lines and arcs to dimension on a 36 tooth gear, for example. And if you consider "real world" components, how often is a thou not precise enough in an assembly? Many thanks!

[JDMather]

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@rataylor wrote:

.... if you consider "real world" components, how often is a thou not precise enough in an assembly? 

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In the real world though you have physical bodies that come in contact.  Doing Contact Sets in the virtual world would be too computationally expensive.  Therefore you pretty much have to have the locations precise. (I have used Tangents before for imprecise holes on imported components, but they are prone to breaking.)  On top of that - when I examine imprecise geometry - it is almost always not what the designer really intended.  (Why would a designer use .xxx-xxxxxxxx for a hole that is intended to be 1/4 inch? Simple oversight, not intentional.)  For some reaon when I post the number 0.xxx-xxxxxxxx gets changed to x.