Shrinkwrap toolset not showing in Inventor Assemble section - is there a way to get it displayed?

[tadeh.hakopian7BNUW]

I want to shrinkwrap some parts for export to Revit but the shrinkwrap tool is not available.

I just installed Inventor Pro 2022 and updated it to the latest release of 2022.1.1 and everything seems fine.

I tried troubleshooting and looking at settings and documentation but I couldn't find anything helpful. 

Is it default hidden when you install Inventor or do I need to install something else to get that tool to show?

I even opened a model assembly file to see if that would show the tool with a context menu but nothing comes up.

Any help to figure out why I can't get shrinkwrap to show would be appreciated. 

Hopefully it is a minor thing but if I have to reinstall everything then I'll try that too.

I have some reference sceenshots below:

Inventor Assemble toolset showing simplification but no shrinkwrap option.

Not even the dropdown on simplification shows anything for shrinkwrap:

In comparison the shrinkwrap tools should show up in that same area like this:

For reference here's the assembly I am using as a test model for the shrinkwrap:

For those not familiar with Shrinkwrap and what it does here's a video going over the basics:

https://www.youtube.com/watch?v=QJFAada1GgA

[TheCADWhisperer]

The name was changed for 2022.

[Bill_Bogan2]

Try Clicking the Simplify tool.

If you cant get what you need there please let us know.

Shrinkwrap can be used from Task Scheduler.

-Bill

[tadeh.hakopian7BNUW]

If the name was changed then what is it referred to now?

Is shrinkwrap toolset just bundled into the simplify toolset?

I thought the options for shrinkwrap would be in Simplification but I don't see that workflow.

These are the toolsets and options I wanted to use but I can't find them anywhere:

[tadeh.hakopian7BNUW]

Is under simplify > create simplified part?:

When I select that I get a menu that pops up asking for a template with only 2 shown by default:

I wanted to access the entire configuration setting but I can't locate it:

Is it still possible to see this menu in Inventor 2022?

[Bill_Bogan2]

Here is the new Simplify command

[tadeh.hakopian7BNUW]

I see how this works now.

The documentation you linked to was helpful in pointing out different methods:

• Assemble tab > Simplification panel > Simplify
• File Export > Export to RVT - for RVT output only
• Environments tab > BIM Content > Simplify panel > Simplify
• Browser: Model State node > New Substitute > Simplify

It looks like the BIM content method gives you an RFA family for Revit and the other methods give you a RVT Revit file.

Is there more information on how these Inventor to Revit RVT/RFA workflows are done?

There seems to be some hints and starting points but not fully built out workflows to explain how to prepare the files and get them ready into Revit with all the content you want and remove the extra stuff you don't want.

FYI - the export to Revit RVT methods crashes the Inventor session even with the simplest parts configurations so I figure there is something I'm neglecting here.

Thanks.

[Bill_Bogan2]

The property panel workflow is from top to bottom. So, you would supply any information you wanted based on each grouping. So, from the top...
Input

• Model state - these are a good way to reduce part count if using a large assembly. You're not, master/primary is fine.
• View - if you have a specific design view you wanted to use, specify it here.
• Podition - if you have a positional representation you want to use, specify it here.

Envelopes - replaces components with boxes. You don't want that, so ignore this group.

Exclude Components

• If you want to exclude small parts (fasteners, pins, etc) then you would specify a size that would encompass all of those you want to remove from the Revit result.
• Click the button to the right of the Exclude field to see what is Included, click again to get back to Excluded parts.

Remove features - if you don't need fillets, chamfers, small holes, etc. you can suppress them wholly or in part (based on size) using the options for each.

Output - specify RVT file. The specify whether you want one "all element" model or a model structured by the top level components. Depends on what you want on the Revit side. Enable updating if you want to be able to update with changes from the Inventor model. 

Try that and see what you get. If you get an error capture your process using "Screencast" and post it here so folks here can help.

[tadeh.hakopian7BNUW]

Thanks Bill. I will experiment with the settings you recommended and follow up if I run into any issues.

[tadeh.hakopian7BNUW]

@Bill_Bogan2 that helped a lot.

I was able to get some models simplified then exported into different Revit formats.

Though I encountered an issue on a model that I'm not sure how to resolve.

It looks like the Inventor importing of an STP file resulted in the model turning sideways:

Here are my STP import settings which are default:

Here is the STP file loaded into Inventor but turned on its side as you can see by the orientation of the door:

It retains this orientation after simplifying and sending it to Revit formats at which point the alignment is challenging to fix.

Is there a way to correct the orientation on Inventor import? A setting that can be used?

I see there is UCS control but that's after the import is finished and a bit confusing to navigate the options.

Is there another way to re-orient the import besides the UCS tool?

 

Thanks

 

[Bill_Bogan2]

Hi tadeh.hakopian7BNUW,

Try this... (see image)

1. Orient the model so you are looking at what you want to be the FRONT view.
2. Right-click the ViewCube to access the context menu.
3. In the context menu, click Set Current View as > Front.

Then, use Simplify command to create the model. If I remember correctly, the command uses the ViewCube orientation and then when creating a Revit file flips it to Z-up.

Let me know if this works, thanks. 

[tadeh.hakopian7BNUW]

@Bill_Bogan2 that view cube switch and apply did the trick!

Here's the Revit family RFA export looking oriented correctly in the Revit family editor.

So now between the STP file import, simplify settings and the view cube alignment I have a workflow to get these models in to a native Revit format.

I need to refine some of the settings for what to exclude and sub-assemblies but that will be trial and error.

One further issue with the RFA export is that the model ends up as one big 3D mass. It looks accurate per the simplify config from Inventor but you can't remove any of the parts or components separately.

For example when I explode the group the family is in the result is just a mass with shape handles:

To your knowledge is there a way to set up the simplify config in Inventor to keep the parts separated into editable pieces in RFA? 

Also note that if you simplify it directly to a Revit RVT file the same thing happens so I think there's something going on with the simplify config that makes the model one big piece after processing it.

Here are the settings I used for simplify from the original STP file and process it before exporting to a Revit native format:

Any advice or suggestions you have for keeping the parts separate on export will be welcome.

 

 

[Bill_Bogan2]

@tadeh.hakopian7BNUW 

The simplify panel looks like you created a normal Inventor file. I suggest reading this topic to help make the selections for the RVT output: https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-9F0E010C-2295-4021-BB77-89C119ACDA1A

If you have already done that and exported a Revit file, which Structure option did you select?

Here's some more info that may help...

[tadeh.hakopian7BNUW]

@Bill_Bogan2 

Thanks for the update on the process for RVT specific outputs.

I tried it based on your configuration and after reading that linked article.

For reference the STP file I am using in Inventor does have nested states and parts within each state:

From that part tree I expected to get similar levels of separation from the exported Revit content.

I configured the Simplify Option to the RVT format per your recommendations after removing a lot of parts I don't need: 

 

I tried both All in one and Top level Element structure modes to see if the results are any different:

 

Both of the Resulting RVT files in Revit ended up as a Generic Model that is one solid block which does not allow you to edit it as an object:

So I got a simplified RVT file with this process but I cannot actually change it in anyway which is a similar scenario to the RFA. The RVT file does not appear to be a Group, Assembly or Family. Just some kind of 3D object.

I noticed that you point to the top level model browser for the completed Revit models in Inventor.

I checked it out and it looks like you can try to edit the simplify settings at that point.

 

Based on the results so far is there a different way to proceed with the RVT or RFA exports so that I can end up with Revit content that is separated into components/parts/families instead of one solid part?

Are there more options in simplify to try out or perhaps even reviewing how to stage the STP file in Inventor from the beginning to make sure all the parts are identified in export?

If I missed anything from your prior post then let me know and I'll go over it again.

Thanks Bill.

[Bill_Bogan2]

Hi tadeh.hakopian7BNUW,

 with respect to the STEP file, 

Is that something you can share with us?

What level of structure/simplification are you looking to get in Inventor?

When you open the file in Revit, what do you want to do with it? 
I want to make sure I have the picture clearly mind.

Thanks.

[PaulMunford]

Hi @tadeh.hakopian7BNUW You might find this class helpful from Autodesk University.

This class shows the new export to Revit workflow:
https://www.autodesk.com/autodesk-university/class/Inventor-Revit-Revit-Project-Export-Inventor-BIM-...


This AU class from last year focuses on the 'AnyCAD' import part of the workflow:
https://www.autodesk.com/autodesk-university/class/Revit-Inventor-BIM-Exchange-Custom-Fabrication-Ha...

Each class has a video, presentation, handout and dataset, so that you can try the workflow out for yourself.

With regard to structure. The Inventor model will always come into Revit in one 'Lump'. The structure options allow you to schedule and tag nested sub components, without having to 'explode' the Converted Inventor model inside Revit.

[tadeh.hakopian7BNUW]

@Bill_Bogan2 

What I want to take from this STP file into RVT is to maintain the 3 main components as separate pieces.

The Frame, Walls and Roof are all distinct components in the STP file and I want them to be simplified and converted to the RVT file in that same distinct set of parts if possible.

Here is the overall file with everything

 

Frame portion

Wall Portion

Roof Portion

When I export these to RVT with Simplify it ends up as one giant lump of a piece without further division or control of the parts:

 

.

Is it possible to use Simplify settings or another setting to keep the parts separate into Revit?

I uploaded the original STP file  without rotation into the post so let me know if that is accessible for you. 

 

[tadeh.hakopian7BNUW]

@PaulMunford thanks for the documents these will be useful.

As for the Inventor Simplify export to RVT I just posted a reply to Bill Bogan referring to how I want to keep the STP file structure distinct after the simplify command.

Based on that post is it possible to simplify it and keep the separated part structure into Revit?

[Bill_Bogan2]

Thank you for the stp file. I'll give this a go in the morning... to see if I can make the output correctly.

[Bill_Bogan2 · Accepted solution]

Hi Tadeh,

Here's the workflow I followed to get three separate components in Revit:

1. Import STEP file into Inventor as a Convert Model
2. For each major component I created a Model State. (Suppressing the other two components)
3. Created a Simplified RVT model for each of the model states.
4. In Revit, Insert tab > Link Revit, select one of the RVT files. Repeat for each model.

   I think this is what you want. It's a few more steps because of the current implementation. 

-Bill