topic Parametric assembly with cross referenced parts in Inventor Forum

Parametric assembly with cross referenced parts

serhanakdeniz — Fri, 02 Jul 2021 22:06:50 GMT

Hi,

Inventor is not happy with my work flow and I get lots of errors if I edit core parameters of my designs.

To explain my work flow,

When I first create a new part in an assembly, I lock it in appropriate position with constraints on elementary planes (xy,yz,zx) either assembly coordinate system or another existed parts' coordinate system and create sketches and features around it which reduces complexity for me.

This works for me most of the time, if I go back the reference file and edit parameters, all assembly gets update and everything is fine. But it only works until at a point where assembly constraints are involved.

I have a design which includes a frame and sheet metal parts that are placed inside and around that frame. And thus, I have many cross reference. I have general dimensions which are set as parameters in the frame reference file, and all other parts are linked to that, and I have sheet metal sketches which other parts' features projected in them. This way, if frame dimensions change, sheet metal parts change accordingly.

Everything is fine and no errors whatsoever until I finish the design and try to iterate with the parameters I created. When I change parameters and model updates, it seems like Inventor calculates something with wrong hyerarchy and this interferes with multiple other cross-part reference, so I get multiple errors. Sometimes after I accept error messages an immediate re-update solves everything, sometimes errors more stubborn and won't disappear. This can be reversed by simply giving original inputs to the parameters but annoys me because I cannot iterate with model.

Any suggestions on that? What am I doing wrong?

Re: Parametric assembly with cross referenced parts

A.Acheson — Sat, 03 Jul 2021 00:21:34 GMT

Is it possible to provide a small sample of the assy and parts linked for update? Without a model to run through it can be hard to identify what is breaking. it maybe a case that certain parameters will need to be before others or to suppress and unsuppress constraints while parts update. If your able to record a screencast this might make it easier also to see what is going on.

Is there any adaptivity involved?

Re: Parametric assembly with cross referenced parts

gcoombridge — Sat, 03 Jul 2021 04:20:45 GMT

Hi @serhanakdeniz, in my opinion cross part references are to be avoided at any cost! There is one exception: when I need to put bolt holes in frame generator members and even then I only project from the frame sketch. It comes down to you appetite for instability I guess (mine is zero 😁)

Have a look at this similar recent post: https://forums.autodesk.com/t5/inventor-forum/adaptivity/td-p/9995165

Skeletal modelling with the derive tool is the workflow I suggest you look into

Re: Parametric assembly with cross referenced parts

SharkDesign — Sat, 03 Jul 2021 05:48:01 GMT

Sounds like you have way too many projected lines. This will usually cause the part to fail because there's too many places for it to go wrong.

If you can drive it all from parameters, use this method.

https://www.youtube.com/watch?v=8qu7jwK9M6k

Re: Parametric assembly with cross referenced parts

serhanakdeniz — Sat, 03 Jul 2021 08:06:22 GMT

Hi Alan,

I can provide whole assembly no problem. Just it is my first thread in Inventor Forums so is it ok if I upload about 20 sheetmetal parts and around 12 frame member all at once?

When I say cross referenced parts, I meant adaptivity. Since I need sheet metal parts to fit into frame members, I have projected edges of frame members or of other sheet metal parts into face sketches. My error messages are not about lost reference, (although I sometimes have that issue too) they are telling me this and that assembly constraint is problematic and needs to be edited but its because Inventor didnot update a part dimension therefore constraint cannot fit. Or vise versa, a constraint did not updated so reference part is not where it should be while part dimension tried to update.

Re: Parametric assembly with cross referenced parts

A.Acheson — Sat, 03 Jul 2021 08:24:29 GMT

@serhanakdeniz

Welcome to the forum. Sure just do a pack and go of the assembly and place in a zip folder and uploaded. If you have Inventor version too so user know if they can open the files. Include some screenshots of the problem areas if you can too in case users can’t open the files and want to chime in.

Re: Parametric assembly with cross referenced parts

serhanakdeniz — Sat, 03 Jul 2021 08:17:17 GMT

Hi James,

Each parts have max 3-4 projected geometry from other parts but in general assembly it sums up of course.

Here, I tried to explain with some screen shots,

Image 1: This is example part and where it stands.

Image 2: The part it must be in touch on right side.

Image 3: The part it must be in touch on right side.

Image 4: How the part defined. It uses the 3 parameters to define the distance between parts in Img 2 and IMg3

Image 5: How it's sketch defined. As you can see it only has 2 reference geometry to define top and bottom points. These are referenced to Img 2 and Img 3 parts top and bottom extremes.

Image 6: How I use parameters menu. I link my all parameters throughout all parts so I can use them where I need.

Re: Parametric assembly with cross referenced parts

serhanakdeniz — Sat, 03 Jul 2021 08:18:15 GMT

and the other ss

Re: Parametric assembly with cross referenced parts

johnsonshiue — Tue, 06 Jul 2021 16:30:38 GMT

Hi! If I understood your request correctly, I think you would be better served using iLogic. The biggest advantage of iLogic is the ability to drive parameters at all levels from the top-level assembly. Without iLogic, you would need to link parameters, or create cross-part reference. These workflows require constant attention to the associative relationship. You need to make sure the drivers and the adaptors (derive) are behaving the way they were intended.

The images don't show much. Please share a simple design you are working on. Forum experts can help take a look.

iLogic is very easy to pick up. Here is a good iLogic collection by our expert elite @S_May.

https://forums.autodesk.com/t5/inventor-customization/collection-of-ilogic-models-for-beginners/td-p/7330801

Many thanks!

Re: Parametric assembly with cross referenced parts

SharkDesign — Tue, 06 Jul 2021 16:36:07 GMT

This is the quickest and easiest way with iLogic.

https://www.youtube.com/watch?v=8qu7jwK9M6k

Re: Parametric assembly with cross referenced parts

serhanakdeniz — Thu, 08 Jul 2021 19:31:58 GMT

Hi,

I suppose you all right that I need to discover about iLogic. I'm a bit reluctant on it since it looks easy in a few parts of assemblies but gets time consuming and confusing with more and more parts.

I really enjoy using Inventor and it's easier and more intuitive than other softwares but I think cross parts references are more successful with Catia V5. Maybe iLogic can change my thoughts.

I mark your post as solution because I really loved the work of @S_May and I'm going to dive into it. Thanks.

Re: Parametric assembly with cross referenced parts

torbjorn_heglum2 — Fri, 09 Jul 2021 06:36:18 GMT

In my opinion you have met one of the shortcomings of frame generator. The tool is is very effective when it comes to creating a frame with members from content center, but if you need additional parts that you want to be associative with your frame this workflow does not support it properly.

iLogic and parameters can help you and make the model more stable, but it can be a lot of work.

You should look into master modelling. Basically you create all you need as bodies in a single part, then you push the parts into an assembly. Associativity within a part is much more reliable than adaptivity, and you can create quite advanced assemblies that doesn't fail on updates.

I think I have placed some examples of Master modelling in this forum.

Torbjørn