Import Inventor 2009 sketch?

[Anonymous]

Is there a way to import an Inventor sketch provided by a product supplier? 

I'm trying to import the following sketch profile, but when it loads into Fusion 360, it is blank:

http://www.minitecframing.com/Products/Aluminum_Profiles/Aluminum_Profile_Catalog_Pages/20.1063_Alum...

(At the top-center of the page it offers three download options. The Solidworks sketch imports blank too.)

[innovatenate · Accepted solution]

The Inventor file only contains a sketch, no 3D geometry. Fusion 360 treats Inventor files similarly to STEP files. Importing an Inventor file would not import the sketches, only the 3D geometry as a "dumb solid." For this case, you could use the STEP file to import 3D geometry. If you would like to create a sketch of the profile, you can use the Project to Sketch command in the sketch menu to create a sketch. Or you may use the direct edit tools, like press/pull to modify the existing 3D geometry (from the STEP file). 

Attached is an exported DWG file from the Inventor sketch in case that helps. Let us know if you have any questions.

Thanks,

[Anonymous]

How do I delete the STEP object used to create the extrusion?

I don't need it after creating a new body or component from a face of the STEP, but A360 won't allow me to delete the STEP object.

Create new project "TEST"

Import STEP file into TEST project

Create new document in TEST project, save it, open it

Drag STEP object into the editor window

Select face on STEP object to use as sketch

Extrude to new body or new component

(at the moment I don't know the difference between a body or component, but the choice doesn't seem to matter for this example. I get the same result below for either choice.)

Name new component "10mm Extrude"

Select STEP object in the browser tree with the chain icon, Delete

Warning: This feature is referenced by other features in the timeline.

Delete anyway. There's nothing indented under the STEP object so I have no idea what that means.

The new object is still visible but now I have an exclamation point in the bottom right corner.

Warning:

   Extrude1:

      Reference Failure:

         Failed to get target occurrence transform.

         The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline.

So how do I get rid of the STEP object?

[jeff_strater]

Hi @Anonymous,

The quick answer is to edit the sketch on the face of the STEP object, select all the geometry, right click and choose "Break Link".  This will break the link between the face of the STEP object and the sketch geometry, which will then allow you to go back and delete the imported geometry.

I'll throw together a quick screencast showing how to do that, and post it here.

Jeff Strater (Fusion development)

[Anonymous]

Hmm, it sort of works, but this leads to another question. What is the difference between Delete and Remove?

Create extrusion.

Select the STEP object in the browser tree, choose Break Link.

Succeeds.

Next I right click on the STEP object, and there are two choices:

- Delete

- Remove

If I choose Delete, it again says

This feature is referenced by other features in the timeline.

If proceed with the Delete I get the same yellow exclamation and the same errors.

If I choose Remove, the STEP object disappears from the browser without any warnings or errors.

Why doesn't Delete mean the same thing as Remove?

Also as a result of this extruding and deleting of the source STEP, the object I have extruded is no longer aligned with the 0,0,0 grid origin in this document. Does this matter for future editing/design purposes, or is it not important?

[jeff_strater]

OK, so my earlier response was only partially correct.  I forgot one critical piece, which actually makes the Break Link even unnecessary.

So, let me step back a bit and explain what's going on.  When you imported the STEP geometry and sketched on the face of it, you created a persistent relationship to that geometry.  The idea is that if you go back and edit the source design, the sketch will update.  There are two sets of relationships here.  The first (and the one I forgot) is the link that the sketch needs to just define the sketch plane.  The second is a reference to each edge of that face, which is used in defining the profile.  That is the reference that the "Break Link" breaks.

So, then, you need to redefine the sketch plane in order to break the sketch plane link.  And, it turns out that if you do that, the references for the sketch lines and arcs are also broken.  So, that's all you need to do.  Here is a screencast:

Now, this video will change the sketch plane to the origin, which will move the component, but you can then move it wherever it is needed

Jeff

[jeff_strater]

Ha!  Our posts crossed in the mail...

Your solution to the problem is also valid.  You did Break Link on the actual imported STEP design.  That works, too.

Next, "delete" vs "remove".  Just between us, I am not fond of the distinction here.  Both of those words, to me, in English, mean the exact same thing!  I tried to argue to get those names changed because they are confusing, but you can't win 'em all...  Here is the difference:  "delete" goes back and deletes the feature that created the object.  Internally we call this "hard delete".  It's as if the object never existed at all.  "remove" inserts a feature in the history that removes the object from the browser, but if you roll back in time, that object will come back to life.  We call this "soft delete" internally.  Soft delete can be useful, if you need to go back to make changes such that the object needs to exist for a while.

Here is another screencast.  I create 3 bodies (ignore the undo in there, I just forgot to check "new body" the first time through).  Then, I select the middle body, and do "remove".  You can see that this inserted a "remove body" feature in the timeline.  Body 2 is gone, but if you roll back, it comes back.  Then, I delete that feature, and show how "delete" works.  Delete goes back and removes the Extrude that created body2.  Which then causes sketch3 to fail, because it can't find its sketch plane.

It's a bit confusing, but hopefully this helps,

Jeff

[Anonymous]

Ok, thank you. I must say, this import process has been so difficult that it reminds me of the learning curve diagram for Dwarf Fortress. 

I am probably going to make a request in the suggestion section to allow direct importing of sketches from Inventor/Solidworks. That would have cut through all this complexity, to just load in the manufacturer's provided sketch and immediately start from there.