Mirroring assembly components issue

[Anonymous]

Hello,

I am working on a parametric design in Inventor 2017 and I have an issue with mirroring a component.

Below is my begin situation:

Begin situation
When I change the length of my conveyor and update it I get the following:

Made some changes
Some parts are, as you see, wrong placed now.

When I open my subassembly and just click and slide over my wrongly placed components it jumps back to it's original position. Below the blue border is my subassembly.

The left leg (with the red circle around it) is mirrored (with the Reuse option) from the right leg.
Is there a solution to this problem or can I somehow update the subassembly without opening it? (I already tried it with an iLogic rule, it doesn't solve this problem).

I hope you can help me with this.

[Thomas_Savage]

Hello @Anonymous

Could you attach your parts and assembly please so i can have a look?

Thanks,

Thomas.

[Anonymous]

Okey here it is. I hope you understand the dutch words in it.

You can change the assembly through the design form in the assembly Parametric Roller Conveyor

[johnsonshiue]

Hi! I took a quick look at the dataset. There are some missing CC parts but they are not relevant to the issue we are discussing here. Anyway, I think this is about how to properly set up assembly constraints. Take a look Pedestal assembly.iam. The components within the assembly are driven by Skeleton rollenbaan.ipt. However, there are grounded parts, which cannot be moved. If I understood how this assembly should work correctly, the components should be constrained to the skeletal part, right? Or, at least they are constrained in a way that the change in skeletal part will propagate to the components.

Many thanks!

[Anonymous]

Yes that's correct, the whole assembly is driven by the skeleton. The parts which are directly created from sketches out of the skeleton (like the right leg) have no problems with the changes. Only the component mirror feature doesn't work properly, so I thought maybe it's just a bug in Inventor?

[johnsonshiue]

Hi! I could be wrong but I don't think I saw a bug. The parts that are not moving accordingly are grounded. As a result, change in the skeletal part would not trigger a move on grounded parts. It is possible I misunderstood the issue. Could you tell me what exact parameter to change in the skeletal part and what exact part is not moving?

Many thanks!

[Anonymous]

The whole assembly is driven by 2 parameters which I added in a form. So when you open the master assembly: Parametric Roller Conveyor.iam and go to the iLogic forms and click on Design you get a window with Aantal_Rollen (quantity of rolls) and Tussenafstand (distance between the rolls). The best is to change the parameter Tussenafstand which increases or decreases the total length of the conveyor. I discovered that when I increased it the parts move along just right and when I decrease it the parts are displaced. The part which doens't move properly is in Pedestal Assembly.iam and I guess it is Pedestal:2 (because 1 is driven by the skeleton). This one is mirrored from Pedestal:1 (reused). Also the adjustment leg is not moving properly, but you can focus on the Pedestal because if that issue is fixed I can easily change the other parts myself. I hope this is clear enough from you. 

P.S. I am not able untill tuesday to open the assembly again, so take your time haha.

[johnsonshiue]

Hi! I think I understand the behavior better now. In Pedestal assembly.iam, Flush:1 fails. The constraint is not needed. You need to add a Mate or Flush constraint between Pedestal:2 and Middle plate pedestal:1 or Middle plate pedestal:2. After that, the assembly will adjust to the change in length properly.

Many thanks!

[kelly.young · Accepted solution]

Hello @Anonymous I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!

Thanks for attaching the assembly parts, much easier to assist. 

To add to what @johnsonshiue states, you have Grounded parts in your sub-assembly that is causing the issues. If you remove the ground and constrain them together and to the base sketch it should function much better. 

It also appears you have the -990 constraint dimension set that doesn't match up with the 900 dimension in the master sketch.

You might consider adding a lines to the SkeletonRollenbaan sketch to locate the MiddlePlatePedestal parts.

Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

This works indeed! So skeletons work fine in the part environment and when you use it in an assembly you should constain to it instead of placing parts grounded at the origin. Thanks!

[kelly.young]

@Anonymous glad you got it figured out, here is some good additional info about skeletal modeling:

Help: Use skeletal modeling

YouTube: The Basics of Skeletal Modeling in Autodesk Inventor Part 1 of 2

AU: Top-Down Design with Autodesk® Inventor™ Using Skeletal Modeling

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

Hi Kelly,

I was looking for a solution to the same problem mentioned by Buwalda.

I noticed I did gound the parts I mirror, now, I did remove the grounding.

But I still can see the parts move to follow as the originals.

Is it possible to reestablish the parts I mirrored or I need to re-do it again?

The file is quite big but if is there a need to send it, please let me know.

Thank you so much for your assistance in this matter.

Sincerely Sam

[johnsonshiue]

Hi! I believe you just need to add assembly constraints (Symmetric) or joints to the mirrored components so that they move according to the source side.

Many thanks!

[Anonymous]

Hi Johnsonshiue,

I did my best to constrain every single piece, Angles, channels, clip angles and bolting,

I think the main issue was that I grounded them all during the mirror process.

After reading your post I realized that, I removed the grounding for all pieces but with no success to retrieve the latest pattern for the new location. I also tried to move them with the FREE MOVE tool but it didn't accept the move. They don't want to forget the previous location.

Kelly Young is also looking into this issue.

But I think there is no way to recover the new constrain location.

But it will be nice to avoid this kind of situation.

Thank you so much for your suggestion although and I will post if support find a solution as well

In the meantime I have to move on and delete them and re do it all over again. not too bad but I don't want to imaging if I had had a bigger model.

Regards,

Sam