topic Re: iPart sketch errors in Inventor Forum

iPart sketch errors

rh8mpo — Mon, 12 Mar 2018 11:12:03 GMT

I have created an iPart with 4 different configurations - these configurations have different features suppressed and some different parameter values. When switching between configurations some of the suppressed sketches trigger error messages - because they reference features that are suppressed.

Although these errors don't cause any problems, I prefer not to have any errors in my models and they are potentially confusing for other users. On other versions of the same model the sketches do not flag up error messages. I can not work out what the difference is between the different versions - can anyone suggest what this might be causing this issue, and how I can eliminate the sketch error messages (without affecting error messages in general)?

Re: iPart sketch errors

Thomas_Savage — Mon, 12 Mar 2018 11:35:24 GMT

Hello @rh8mpo

Could you attach your model please?

And what version of Inventor are you using>

Thanks,

Thomas.

Re: iPart sketch errors

rh8mpo — Mon, 12 Mar 2018 11:43:04 GMT

Thanks for the response - I am using Inventor 2014.

Please find attached two versions of the model:

- VC version throws up sketch error messages, this was developed from the other version that doesn't

Re: iPart sketch errors

Mark.Lancaster — Mon, 12 Mar 2018 11:45:29 GMT

@rh8mpo

I would suggest that you don't project or use geometry of features/sketches that get suppressed in your iPart table. In addition just because it may seem its not impacting your design, failed geometry will always cause issues down the road and should always be resolved.

Re: iPart sketch errors

rh8mpo — Mon, 12 Mar 2018 11:56:10 GMT

Thanks for the response - it might be possible to calculate the reference points instead of using the resulting features - will give it a try

Re: iPart sketch errors

rh8mpo — Mon, 12 Mar 2018 12:19:34 GMT

I've just resolved one of the sketch errors by calculating the reference point - pretty sure the same approach will work on the other errors.

Re: iPart sketch errors

rh8mpo — Mon, 12 Mar 2018 15:03:05 GMT

Further to my last message - I've now resolved all the broken sketches by either calculating the reference point, or referencing sketches instead of geometry - thanks for the nudge in the right direction

Re: iPart sketch errors

MakkaPakka — Fri, 18 May 2018 08:37:21 GMT

Hi, I am experiencing a similar problem with an iPart. I am suppressing two features in one member. They are the last two independent solids in the browser. One feature (a sweep) is dependent off the other (circumferential edge of curved plate). I can understand why you might get an error if an unsupressed feature referenced one of the two suppressed features. But if the both features being suppressed are just dependent one on the other, why should an error reported? Its as if Inventor is still calculating the secondary feature despite it being suppressed, then finding an error because the primary referenced feature is suppressed. I note that the error is reported in the automatically generated 3D sketch which represents the edge of the curved plate.

Re: iPart sketch errors

johnsonshiue — Fri, 18 May 2018 15:10:20 GMT

Hi! This sounds like a file specific behavior. Could you share it here or send it to me directly (johnson.shiue@autodesk.com)? There should be a logical reason behind the failure.

Many thanks!

Re: iPart sketch errors

MakkaPakka — Mon, 21 May 2018 11:08:37 GMT

Hi please see file attached

Re: iPart sketch errors

johnsonshiue — Mon, 21 May 2018 14:34:46 GMT

Hi! I took a quick look at the file. Could you explain to me that why each feature creates a new solid body? What is the purpose? Shouldn't all the features act on the same body?

Many thanks!

Re: iPart sketch errors

swalton — Mon, 21 May 2018 15:06:54 GMT

The error in Sketch 10 is because the Pad feature is suppressed. Once the Pad feature is resumed, the projected edges from the Pad feature in Sketch 10 can be re-computed and the issue is resolved.

I don't think that this is not a geometry or file specific issue, instead it is a basic workflow assumption made by the Inventor developers years ago.

As I understand it, Inventor always computes each sketch in a part model, even if the driven feature is suppressed. I think this goes back to the idea that the sketch is the parent of a feature, not a child.

In my perfect world, when I suppress the "Pad" feature, Sketch 4, Fillet3, Sweep11, Sketch10 and 3d Sketch10 would all be suppressed. All these additional features in the model tree rely on geometry created by the "Pad" feature. If I did not want these dependent features to be suppressed, I would want a workflow to change the geometry references of the dependent features. Creo does this, but I'm sure the workflow could be smoother.

@johnsonshiue, is there a way to stop computation of a sketch when the driven feature is suppressed? I can see issues with a Shared Sketch, but if a sketch is used in only one feature, I don't see a reason to compute it.

Re: iPart sketch errors

johnsonshiue — Mon, 21 May 2018 18:18:57 GMT

Hi! Steve,

I can easily reproduce the behavior. And, yes, it is a legacy behavior. But, there are special conditions leading to the behavior. The sketch has to have dependency on a solid body, which is also suppressed along with the body generating features. In this case, Sketch10 and 3D Sketch10 both have dependency on Solid5. When Pad and Fillet3 are suppressed, Solid5 will not exist and the two sketches will error out. If the whole part has only one solid body, the issue will not occur. This is why I asked OP if doing multiple solids is really needed here.

Certainly, there is room for improvement. I personally think the sketch warning is unnecessary. It should simply work as if the entire part has one solid. Let me work with the project team and see if we can change the behavior easily.

Many thanks!

Re: iPart sketch errors

Tom_Sturtevant — Mon, 21 May 2018 19:52:17 GMT

Hi Johnson & Steve,

I’m going to side with Steve on this. The (2D) Sketch10 and 3D Sketch10 projections are of specific edges and/or faces of the solid. When the Pad and Fillet are suppressed those edges/faces are not created and the projection fails. I did try joining all features into a single solid and still see the error.

The possible ways I see to get around this are:

Move the stop node above the Pad feature. But this is not supported through the iPart table…
Use sketch-to-sketch projection rather than edge-to-sketch projection. This should not be too difficult with (2D) Sketch10 but is not an option for 3D Sketch 10.
Model the Pad (including fillets) as a surface and project edges from the surface body into the 3D sketch.

I’ll attach the surface example (and the failing single-solid example).

Hope that helps…

T.0.M.

Re: iPart sketch errors

MakkaPakka — Tue, 22 May 2018 07:27:27 GMT

Hi Johnson

Thank you for looking at this. The reason for the separate bodies is that two solids represent weld fillets. I want these to come through into the .idw as hatched features in a section that can apply a solid hatch to. Depending on which iPart is generated (I only sent one size in the table), the weld features are sized to suit the plate thickness. I know that strictly speaking this is not the correct inventor workflow for a weldment but I wanted to keep the parts simple i.e. one part with multiple bodies rather than separate parts bought together into a weldment. If I did that, Inventor welds would have to be applied in each case and I'm not sure that a weldment iAssembly would be as self contained and simple to set up as this single part method.

Re: iPart sketch errors

Tom_Sturtevant — Tue, 22 May 2018 17:05:07 GMT

Hi MakkaPakka,

If you have not already, take a look at Lifting Lug_Surfaces.ipt that I attached above. It definitely adds some complexity to the part recipe but it is a possible way to keep the sketch from becoming sick.

Thanks,

T.0.M.

Re: iPart sketch errors

MakkaPakka — Wed, 30 May 2018 13:38:19 GMT

Hi Tom

Thanks for posting the files. The surface one is interesting, I have not used any of the surface modeling tools so far. I may be wrong but does any kind of surface modeling have an effect on mass properties? Since my last post I tried another approach by bending a flat plate for the pad feature and its associated chamfered edge. When suppressing these I get no residual errors. This has worked well. At least its been a lesson for me in what to consider before starting to model iPart features that need to be supressed. Thanks to all for thoughts on this one.