Inventor 2016 AnyCAD Technology

Posted on August 19, 2015 by Mark Lancaster, Synergis Manufacturing Product Support Specialist
I have been asked numerous times, “What’s possible with the AnyCAD function within Inventor 2016?” Think about the term “AnyCAD”, doesn’t it seem like Inventor 2016 is wide open to work with any CAD file/format/platform that may be out there? So today I want to clarify what this technology is actually all about.
The AnyCAD technology was incorporated in the 2016 version so Inventor users can work with other popular CAD applications without the need to remodel or re-import files that were created by these applications. With a couple of mouse clicks you can now maintain a relationship back to the native CAD application and start designing using this shared information. When changes occur in the native CAD application, guess what happens in your Inventor model? The design data from the other CAD application will update in your Inventor model.
AnyCAD has basically two capabilities:

1. The first part allows the user to create a reference model within Inventor
2. The second aspect creates a converted model

So let’s start out by reviewing what a reference model is.

Reference Model

In the past, when you opened a non-Inventor CAD file created by your co-worker (let’s say they were using SOLIDWORKS), Inventor would convert it to an appropriate (Inventor) file format. When changes were made by your co-worker, you had to follow the same process to update your Inventor model and most likely you spent time rebuilding your model every time this occurred.
Now with Inventor 2016 and the AnyCAD technology, you are able to maintain the relationship between your model and the other CAD application. This workflow is demonstrated in an Autodesk Screencast I created about the “The Power of AnyCAD”.
The reference model interface will only work with the following CAD application/versions:

• SOLIDWORKS (version 2011 Plus-2015)
• PTC Creo (version 1.0-3.0)
• Autodesk Alias (version V10 and later)
• Catia (version VA and R6-V5 6R2014)
• NX (version UG V12-NX9)
• Pro/Engineer Wildfire (version up to Wildfire 5.0)

To create a reference model in your assembly, simply select Place Imported CAD files from the Place Component section of the Assemble ribbon tab. An alternative method is to either select the normal Place Component function or you can drag/drop the (imported) CAD file directly into your Inventor model.
Helpful tip #1: In those cases where you want the imported CAD file to be the first component in your assembly you can also use the normal Inventor Open or Open/Import CAD Files menu selection to automatically start your assembly and create/ground the reference model.
Next, navigate and select where the file is located and then define your import type. In my case, I want to select the reference model option in order to maintain the relationship to the SOLIDWORKS file that was given to me by my co-worker.
From there you can select which geometry (object fillers) will be brought in and the units that will be used.
Helpful tip #2: If you want to preview the imported CAD file before placement, pick the “Select” tab and the “Load Model” button.
Also, if you were importing an assembly, you can simply select which sub-components to exclude (or include) using the same method listed above.
Once the SOLIDWORKS part (or assembly) is brought into your model, you will notice it appears in the Inventor browser window/tree as an Inventor part (or assembly) icon with the imported arrow symbol.
If changes are now made to my referenced SOLIDWORKS file, the Inventor model will also update. Now that we created a reference model using the AnyCAD technology lets switch over and talk about the converted model aspect of it.

Converted Model

Prior to Inventor 2016, any supported file type brought into Inventor was considered a converted model. So there really is nothing new about this aspect of the AnyCAD technology except for the three minor changes that I will list below.  File types of IGES, STEP, Revit, SAT, and etc. are still imported into Inventor and converted to an appropriate Inventor file type. However, CAD models that belong to SOLIDWORKS, PRO/E, and etc. can still be converted to an Inventor file just like you could in the past.
Changes:

1. In the previous versions of Inventor you used the “OPTION” button on the open dialog to select your import options. In 2016, the import options are accomplished through the “Import” dialog after you select your file. The options presented in this dialog are solely based on the file type/configuration you are importing.
2. When importing prior to Inventor 2016, the stored location was based on the settings in your Inventor project file and/or the Import Option dialog. In Inventor 2016, the file name and location can now be defined via the “Import” dialog or at a later time.
3. In Inventor 2016, you can now preview the imported file using the “Select” tab/load model as described earlier in this article.

 
Now that I have gone over the capabilities of the AnyCAD technology, you may have some additional questions regarding it. Here are some important FAQs about AnyCAD:

• If a vendor of ours provides me with a SOLIDWORKS file of their standard part (which may never change) do I have to make a reference model within Inventor?
  • The answer is no but it is your choice. When you import certain file types (or your SOLIDWORKS file), you have the option to define it as a referenced or converted model.
• I created a reference model to a Pro/E file and our Pro/E designer is out. Can I make changes to it in Inventor?
  • The answer is no. A reference model is controlled by the native application and editing any aspect of the reference is not permitted. However, if you right mouse click on the reference model in the browser window you can change its import options.
• Will any of my constraints fail when my co-worker modifies the files that I referenced into model?
  • It is possible, but it all depends on what modifications are being made to the referenced CAD file.
• In the Import dialog/Select tab, I am able to exclude components in the assembly that I am referencing. Can I include them later on if needed?
  • The answer is yes. At anytime you can right mouse click on your referenced model in the browser tree, edit the import options, and pick the “SELECT” tab to change which components are excluded/included.
• What happens if my co-worker changes the location of the native file I am referencing to? Will Inventor find it?
  • The answer is yes and no.
    • Yes – If the link to the reference model was suppressed when you last saved your model, Inventor will continue to load your model no matter where the reference files are located. Basically at this point your model only contains a snapshot of the referenced information when the link was originally suppressed.
    • No – Most likely, Inventor will issue the resolved link dialog to relocate the reference model. But it will all depend on if the new location is part of the search area or not for Inventor.
• Sometimes when I get a STEP file I just want to look at it. Does that mean I will need to provide a file name and location just to view it?
  • The answer is no. The file name and location field is optional in the Import dialog box.
• When I reference an assembly from a supported CAD application, will it appear as a sub-assembly in my Inventor BOM?
  • The answer is yes.
• It appears AnyCAD will help our Inventor users create designs by referencing data from other supported CAD applications we have in our company. I have two questions regarding this.
  • Sometimes the information we receive from the other division needs to be referenced into our model but not included in our BOM. How can we accomplish this?
    • Simply right mouse clicking on the reference model is the browser tree, select BOM structure and setting it “REFERENCE”
  • If the other division is already applying BOM information in the native CAD application, is it possible for Inventor to use that information or do I have to redo it?
    • First of all, a reference model is under the control of the native application and cannot be modified within Inventor. Second, the information from the native application gets carried over based on the property mappings you have in place for Inventor 2016. These mappings (XML format) can be found in your design data location under the “Import Properties” sub-folder.
• If I reference a SOLIDWORKS assembly into my Inventor model and my co-worker only modifies a sub-component of it, will the referenced sub-component update in my model?
  • At this time the answer is yes and no. However, it appears this workflow causes an issue with the Inventor browser tree and BOM structure. Although Inventor sees a change, the reference component will disappear from the graphic window when the update is applied to your model. This workflow issue has been submitted to Autodesk for resolution.
• If I reference a model in Inventor or create a converted one, can I change it later on?
  •  The answer is no. Although with a reference model you can right mouse click and edit the import options, changing how it was originally imported is not possible.
• At any point can I break the link to the reference model?
  • The answer is yes. If you right mouse click on your reference model in the Inventor browser window, you can either break or suppress/un-suppress the link. When you suppress the link, the link is maintained but the reference model will not update. When the link is un-suppressed, the relationship is re-established and any changes since the link was suppressed will be incorporated. However, if you break the link, then the reference model is converted to an appropriate Inventor file type and the relationship is forever lost.
• We often pack n go our Inventor models and send them to others located outside of our company. What happens when you pack n go an Inventor model that contains a reference to another CAD application?
  • The components that are referenced into your model are included in the pack n go destination.
• Our sister company in Europe uses CATIA and AnyCAD will finally help us to maintain that relationship with those types of design files.  However, we use Vault here in the states and I was wondering what happens to files that are referenced into our model? Would they get checked into Vault as well?
  • The answer to your question is yes and no. If the files that make up the reference structure are within the Vault workspace scope, they will be included in the check in operation. If they fall outside that scope, they will not check in and Vault will issue a message related to that. At that point, your entire assembly will also not be able to be checked in and you must resolve the location issue before that can happen.
• The information you have already provided to us about AnyCAD is very helpful. However is there a quick guide for the AnyCAD technology that I can post or share with my user?
  • For the AnyCAD technology, I follow this one simple image. Anything left or right of the center image can be imported as a referenced or converted model. Any file types above or below it will always be imported and converted to an appropriate Inventor file type.

Hopefully the information and answers to these previously asked AnyCAD questions will help you understand what is possible within the AnyCAD technology. If you have any questions about this capability in Inventor 2016 please feel free to contact us.
Until next time,
Mark Lancaster
Mark Lancaster joined us back in August 2013. His most previous experience is as the CAD Design Manager of Pall Corporation, one of our long time customers. In that position, he was responsible for workstation optimization and design management, established uniform standards for the local and global offices, and developed global systems to control and manage their design data.