UnfoldFeature.StationaryFace

[florian_wenzel]

Hi, 

i try to make a Unfold of a Solid Profile in Autodesk Inventor.

Normal it works fine.

i Mean, i create a Solid Model, then a Convert it to SheetMetal.

I define a Thickness of the Material, and it works, usually.

The Problem  is, that sometimes does not appear the Stationary Face, and im not able to make the Unfold.

I Have 2 Profile, one of them work Properly, i define the Thickness and i'm able to select the Stationary Face.

The Second Profile, has the Problem, that the Stationary Face does not apper.

Is there any Possibility to manually create a Stationary Face, with API or with VisualStudio (via StandaloneExe).

First Profile - With Stationary Face

SECOND PROFILE

without Stationary Face.

Any Suggestion.

Thanks

[adam.nagy]

If you can figure out programmatically which face should be the StationaryFace then you could generate the UnfoldFeature like this - this VBA code assumes that the the relevant face is already selected in the UI:

Sub UnfoldFeatureTest()
  Dim doc As PartDocument
  Set doc = ThisApplication.ActiveDocument
  
  Dim cd As SheetMetalComponentDefinition
  Set cd = doc.ComponentDefinition
  
  Dim smf As SheetMetalFeatures
  Set smf = cd.Features
 
  Call smf.UnfoldFeatures.Add(doc.SelectSet(1))
End Sub

[florian_wenzel]

Hi,

Thanks for your Answer.

It works, when i select manually the Stationary Face, then it make a Unfold.

The Problem is, that it work not always.

[florian_wenzel]

The Problem is, that sometimes does not appear the Stationary Face, and im not able to make the Unfold.

I Have 2 Profile, one of them work Properly, i define the Thickness and i'm able to select the Stationary Face.

The Second Profile, has the Problem, that the Stationary Face does not apper.

I define the Thickness 32mm, this is the max width of the Profile, not the Bridge 10,4mm.

And it Works.

In this case, we use 3D Model from other CAD Program (HiCAD).

So it looks so, that we import a STP file in Inventor, and make with Inventor Unfold.

In Attachment you can finde STP File which i try to make the Unfold.

Working Profiles:

Konstruktion1.1

Konstruktion2.1

Not Working Profiles:

Konstruktion3.1 (This Profile has a Diffrent Thickness at the hole Lenght. The Tolearace is about 0,00013 mm)

Konstruktion3.20 (This Profile has at the Hole Lenght the same Thickness 32mm (bridge 10,4mm)

And now:

Konstruktion3.33 is the Same Profile like Konstruktion 3.20, with this Diffrence, that is without Holes, and it Works Fine.

I suspect that there are some criteria in the Function that make the Stationary Face not appear.
Can i get the Sample of the UnfoldFeature, for example if i willl be the member of Autodesk Developer Network?

[florian_wenzel]

Konstruktion3.20

Konstruktion3.33

[adam.nagy · Accepted solution]

Does the VBA code fail for the same models where the Unfold feature does not offer faces for Stationary Reference?

If so, I assume Inventor's solver has some issues with the model when it comes to unfolding.

The Inventor API can only be used to automate what the product can do - if the product has issue with something, the API will not be of help. 

I'm wondering if I should try to move this post to the Product Support forum, where more people would have a look.

[florian_wenzel]

hi,

"Does the VBA code fail for the same models where the Unfold feature does not offer faces for Stationary Reference?"
The VBA code works Fine with this Profile, which appear the Stationary Face.

By the other Profile, where the Stationary Face does not appear, VBA code doesn't work

"If so, I assume Inventor's solver has some issues with the model when it comes to unfolding."
Yes, i think so.
Is a possibility to get the UnfoldFeature  as Code?

I think, that STP File are maybe Corrupt for this Feature.
They are good to have a Solid Model, but when it comes to Unfold, they make a Problem.
For Example, when i deactivad some of the Holes with Pattern, then it works Fine.

For Example:

Profile: "Brass Cover Inside Bottom28" is Working Fine (also with the VBA code)

Profile: "Brass Cover Inside Bottom30" is not Working (also with the VBA code)

i dont know, maybe some Brep issues wit Exporting to STP, and the Feature Function trow it out.

[florian_wenzel]

ok, lets hope someone help me

[Hochenauer · Accepted solution]

Hi Florian,

it comes down to the model quality of the imported part (or the quality of the model defined by the step file). 
The tolerance you report leads to issues if there is adjacent geometry in the area. We can have our modeling experts take a look if that can be tweaked, but an inaccurate model usually leads to issues with downstream modeling operations.

Kind regards,

Gerald

[Hochenauer · Accepted solution]

On second look, we can create a flat pattern if we preselect the "bend" face. We should be able to help the unfold command with a preselection as well. I will ask our QA to evaluate and maybe create a story to allow that in the future.

Gerald

[florian_wenzel]

Hi,

you mean this Feature? 

unfortunately that doesn't help.

I think in this Feature is a Checklist, and when is a small issues, that the StationaryFace does not appear.

[florian_wenzel]

Another try:

i open the File in Rhino, 

then save as STP ver. AP214 or AP203

Import in Inventor.

And, now appear the StationaryFace, but i get a Error when i select the bend surface.

Error: Calculate error

So, this is not only the Stationary Face.

Something else make the issues.

Is there any possibility to overjump the checking from UnfoldFeature?

[florian_wenzel · Accepted solution]

ok,

it works!

It is very likely that it is due to the quality of the STP file. Because if the geometry is created in Inventor, then it works, so in my opinion it must be the data transfer. The geometry must correspond to the specifications of Inventor, otherwise it does not work.

Solution:

STP Version AP214 with ParametricCurves

[florian_wenzel]

Hi,

new STP files