Model State - Sketch Doctor Issues

[jwente123]

When creating new model states to suppress features on a part, depending on what is suppressed, can cause the sketch doctor to show errors in the part due to missing sketch faces, missing referenced geometry, etc. Is there any way for the design doctor to ignore suppressed features, or ignore the model states and only detect the master state?

I know we have other users at our company that will see the error and think they need to fix something, which will just cause more problems.

Just curious if anyone else is seeing this issue and what they are doing to resolve it.

Below is an example of a plate and a model state for the burnout in a pre-machined state.

When the new model state is selected, the sketch errors appear.

[gmarken]

This is probably not the best solution but you could try positional representations. Suppress the mates there.

[johnsonshiue]

Hi Jeff,

I think I know what you are talking about. This behavior actually has nothing to do with Model States. It is related to the so-called soft feature dependency and inability to suppress a sketch. Sketch6 has a dimensional constraint to a projected edge from Hole1. When Hole1 is suppressed, the projected edge loses it s source and Sketch3 has sick sketch geometry.

To avoid this behavior, you may want to remove such soft dependency. Essentially, Sketch3 will be driven by a parameter shared with Sketch2.

Many thanks!

[MichaelBowditch]

I am having the same issue, this almost makes the Model State feature completely useless depending on how you are designing the part. My understanding was that using various Model States would allow for part revisions/stages to be included within 1 part file, unless we have a crystal ball and can predict what changes/revisions will be made in the future then how does this make sense. The only way to avoid the errors would be to go through the new features and adjust each dimension to avoid the relationships causing them. Currently I am finding it much more productive to just copy the part and continue the design with a new part number to avoid this.

[IgorMir]

The way I see it is -  much drummed up "Model state" is nothing more than re-branded iPart. To avoid the nuisance of individual sketch getting sick - the shared sketch should be used for defining a follow up geometry instead. That way the features are not relying on the projected model geometry, which can be suppressed in some other versions of the part. 
Cheers,

Igor.

[NorthernCADMonkey]

So just getting to model states as we did a late upgrade.

It has been less than useful and this makes it worse.

I agree this makes model states useless if you can't ever model anything with projected edges or geometry. Which are two big parts of Inventor.

I also can not have my design group just ignore the design doctor warnings. It is part of the check that the design team needs to do before submitting work that there is no errors, and full constraints.

I can't have a bunch of parts that error out when in other assemblies or in a different model state. 

Why is there nothing being done to address the sketch, reference or otherwise not being suppressed when its parent feature is. 

Why can I roll back the model in the browser to the same spot as the feature / sketch that when suppressed in model states and that causes no errors.

At this point all model states is doing is creating more issues than providing a benefit.

[BDCollett]

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@NorthernCADMonkey wrote:

So just getting to model states as we did a late upgrade.

It has been less than useful and this makes it worse.

I agree this makes model states useless if you can't ever model anything with projected edges or geometry. Which are two big parts of Inventor.

I also can not have my design group just ignore the design doctor warnings. It is part of the check that the design team needs to do before submitting work that there is no errors, and full constraints.

I can't have a bunch of parts that error out when in other assemblies or in a different model state. 

Why is there nothing being done to address the sketch, reference or otherwise not being suppressed when its parent feature is. 

Why can I roll back the model in the browser to the same spot as the feature / sketch that when suppressed in model states and that causes no errors.

At this point all model states is doing is creating more issues than providing a benefit.

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It is frustrating but until they work out a way to deal with this you can add features to fill in or remove geometry instead of suppressing.

Otherwise, project sketch geometry instead of feature (which should be done as much as possible anyway)

Model States are an amazing addition, they might just require some better modelling practices to use them effectively. 

[johnsonshiue]

Hi Folks,

The trouble with Model States, iPart, and iAssembly is about the ability to manage the soft dependency on the table. In this case, the sketch geometry or sketch coordinate partially depend on a parent feature. Instead of being suppressed, the sketch stays computed but with sick geometry.

To build your model more friendly to Model States, iPart, iAssembly, you may want to make sure the soft dependency is reduced to the minimum, particular for the features you like to configure (drive) on the table. You may want to create UCS or workplane to avoid such dependency.

Many thanks!

[NorthernCADMonkey]

Ok fair enough, I understand the issue is soft dependencies, but saying don't model / sketch / have soft dependencies in your entire model is not a realistic fix. My team is all experienced inventor users and well aware of how sketches, features, placed features ect should be created in order to have best practice / stable models. This is not a bad modeling / user technique issue.

If every sketch / feature has to be independent, individual work planes for sketches, no relations for previous features, no relations to edges or holes of previous features .......ect ect.... then this is a pretty unusable feature.  

The big thing we were looking to implement with the upgrade to 2023 and model states was to be able to show a base "blank" billet feature then the stages of it being machined. This is not really even creating configurations. This is basically just wanting to be able to show the part in the sequential modeling steps, in order of creation in the tree, just like rolling the model up / down the browser tree. It seems pretty unbelievable that we can't even have a model state that only used the first sketch / revolved feature at the top of the model tree with every other feature below it suppressed but still cause an error.

[kimK7B54]

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@johnsonshiue wrote:

Hi Jeff,

I think I know what you are talking about. This behavior actually has nothing to do with Model States. It is related to the so-called soft feature dependency and inability to suppress a sketch. Sketch6 has a dimensional constraint to a projected edge from Hole1. When Hole1 is suppressed, the projected edge loses it s source and Sketch3 has sick sketch geometry.

To avoid this behavior, you may want to remove such soft dependency. Essentially, Sketch3 will be driven by a parameter shared with Sketch2.

Many thanks!

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The best solution would be for Autodesk to change this so the sketch(s) in question can be suppressed when not being used.  If Inventor were to ignore unused sketches then it would not know there was a missing projected edge, etc.  This, so far, has been the biggest headache with model states. (aside from my user error of forgetting to select/deselect "edit factory scope" when editing)