'Getting Started with Model States' AU2021 class: Your Questions Answered

Hi Everyone, 

Firstly "Thank You"! I have taught a number of classes at Autodesk University over the years and often the interest in the MFG classes were a little low. But wow, not this year! My AU2021 class was focused on the new Model States functionality in Inventor 2022. I certainly picked a great topic. I had over 550 register for the class and 70+ connect with me directly during and after the class. So thanks for voting for my class and attending. If you didn't get the chance to attend the conference "live",  the recorded session is posted to the Autodesk University site where you can watch the replay and download my handout to help get you started with Model States (Click Here). 

I had so many questions during the Q&A session that I couldn't answer them all and I promised a blog. Here you go!

I hope to see everyone in person next year at AU2022.

 

QUESTION - Do you have to renumber the BOM for different Model States? If you suppress item #3 in a 5 part assembly will the BOM show 1,2,4,5 or 1,2,3,4?

ANSWER -  The Item numbers in the BOM do not automatically renumber for any Model States that don’t have components displayed. By default, the Parts List will still show 0 Qty for the components that are suppressed so the item number remains.

 

QUESTION - Is there a Filter to turn off visibility of '0' quantity parts?

ANSWER – There is not a filter for Model States that turns off the '0' quantity parts. This article on the AKN suggests a couple of workarounds that you may want to look at. 

 

QUESTION - How does iLogic cope with all these changes?

ANSWER – iLogic has a few new snippets in 2022 that allow you to activate Model States in a file (Active Model State ) or replace a Model State version in an assembly (Replace with Model State). Both of these are listed in the Components (classic) category. Additionally, you can add specific Model State versions when adding components using the Add Component with Model States snippet in the iLogic Assemblies/Components category.

 

QUESTION - Many companies have problems with the BOM using the LOD because it does not remove the parts that are suppressed. Is there anything new in the BOM in the assembly environment with Model States? Works as a drawing as you showed?

ANSWER – Unfortunately, this seems to still be the case with Model States. The suppressed components will show in the BOM with zero quantity. A couple workarounds are included in this article published to the AKN. https://forums.autodesk.com/t5/inventor-forum/model-states-bom-0-quantity/m-p/10298834#M827047

 

QUESTION - Please address the automatic conversion of LODs to Model States. How does it work and affect existing drawings. I'm concerned about damaging legacy data.

ANSWER – If you have LODs and no iParts, all of your LODs will be converted automatically by Inventor into Model States. I have not done this on a large scale so I would certainly look at testing your files once the data is migrated to 2022. If you have iParts/iAssemblies in your files your LODs will be converted to Design Views. Any suppressed components would have their visibility turned off in the Design View. I would recommend searching “Model States" on the AKN (on the Autodesk Inventor forum) as I see a number of customer posts on this that Autodesk has replied to, so it might give you further insight. Click here for a post I found interesting. 

 

QUESTION - Is the BOM or parts list updated when a Model State changes?

ANSWER – Yes, the BOM/Parts List is updated with a Model State change. In fact, you will be prompted that this is happening.

 

QUESTION - Does the Model State remain shown in the Display Name of a component if the component gets renamed by the user? 

ANSWER – I tested this and when a component is renamed in the model browser, the Model State name still is appended to the name if a Model State is activated.

 

QUESTION - You say the iParts and iAssemblies are "still available" in 2022. Speaking for a company that has thousands of these types of files, is there discussion about ending this feature in Inventor?

ANSWER – As I do not work for Autodesk I cannot speak to this.

 

QUESTION - Can you suppress/unsuppress sketches in a model state?

ANSWER –Sketches cannot be controlled with the Suppress command. Their visibility of a sketch is either on or off in the entire model. So you can’t control it with Model States.

 

QUESTION - Should we re-create our existing template files (.ipt and .iam) to take advantage of Model States?

ANSWER – No, this does not have to be done. The activation of Model States is software functionality and not tied to a template.

 

QUESTION - Does the mass remain constant with the way you used Model State to generate the Substitute?

ANSWER – Yes, the simplified substitute maintains the source geometry’s mass.

 

QUESTION - Is there a workflow to convert an iPart to a Model State?

ANSWER – As I discussed in my class, this is currently a manual process. I would recommend reviewing the iPart table in Excel and then using that to reference in the creation of the new model states.

 

QUESTION - Can a new feature be added to a single Model State that won't show up at all in the other Model States (not just suppressing a feature)? For instance, for a model of a wire, being able to have a Model State to show the overall straight length of the wire, and a Model State to show the wire modeled in the shape that it will be in an assembly.

ANSWER – Yes, you can create features in specific Model States and not have them show in others. Ultimately, the feature is still added to the model browser for the Master and all other Model States (non-active) are shown as suppressed in all but the one that the feature was created in.

 

QUESTION - So can you have a Model State that can change iProperties per state? For example, have a pressure gauge some geometry but the only thing that changes is the range of pressure measured. If you place it from a Library search path are they editable or would you have to have all the ranges put in the Model State part file?

ANSWER – Yes, this is possible. With the Model State active, right-click on the file name to open the iProperties dialog box and modify the properties as required. I recommend that once you customize the iProperties that you want to vary in each Model State, that you edit via Spreadsheet to easily modify the remaining while in a table. I did this in my class demo if you would like to review it.

 

QUESTION - Is there a limitation on the number of Model States within a single part or assembly?

ANSWER – I am not 100% sure on this, so I do not want to answer and provide incorrect information. I would recommend that you post a question in the Autodesk Inventor Discussion Forum. Autodesk employees follow the questions and can provide an answer on this.

 

QUESTION - Is there any public news about enabling Model States with Vault Pro and not using Items?

ANSWER – As of Vault 2022, in order to have Vault recognize the properties in each Model States, items must be used in Vault. Click here for a good article about Vault and Model States.  

 

QUESTION - Does this change affect how we create custom content and publish to content center?

ANSWER –  I have not tested this, but in reading the following AKN article (Model State - Inventor 2022 - Autodesk Community - Inventor) there is mention by Paul Munford of Autodesk that for adding libraries to content center that you will want to continue using iParts. I would suggest asking further questions on the planned workflow to Autodesk on this discussion panel.

 

QUESTION - I like the idea of not having all these extra files like iParts creates. If we manually convert to Model States from iParts, should we delete all the old extra files created in the Vault from the iPart creations?

ANSWER – Vault is not my specialty, therefore I would recommend speaking with your reseller or post a question on the Autodesk Inventor Discussion Forum, where Autodesk can reply.

 

QUESTION - In Vault when you assign an assembly to an item with multiple Model States with different part numbers, does it create multiple items for each of the part numbers?

ANSWER – The following AKN article has a section on assigning items that you might find useful. You will need your Vault Professional setup to include items. 

 

QUESTION - Will iParts/iAssemblies disappear in the future? We are using a PDM system other than Vault. BOM is based on file structure, so I guess with Model States we will not be able to extract a BOM from 1 file?

ANSWER – If the system can’t recognize that components in the model browser are suppressed, then I suspect you are correct and the BOM will be for the Master.

 

QUESTION - The disadvantage of iParts/iAssemblies was that the Excel spreadsheets were loaded into memory and slowed down your system. How do Model States do this? Does it still load Excel in the background?

ANSWER – Model States do leverage the use of spreadsheets as well. I suspect that it likely will need to load. I have noticed that the first time you create a Model State in a file it does take longer to create; I suspect because it is creating the spreadsheet. This might be another question that would be good to direct to Autodesk on the Autodesk Inventor Discussion Forum.

 

QUESTION - Do Model States work with Content Center?

ANSWER – I would not recommend this workflow. For specific questions on what Autodesk has tested, I would post to the Autodesk Inventor Discussion Forum.

 

QUESTION - Is it necessary to place all Model State views in a drawing to be able to generate the table with all the variants? Especially assemblies.

ANSWER – No, you do not need to place all Model States in the drawing in order to generate the General Table that lists all the Model States. I did this in my demo, but it is not a requirement.

 

QUESTION - Is there a way to assign a MATERIAL to a body in a multiple body part file so to get a better weight and COG calculation?

ANSWER – No, this is not possible. The material is assigned to model and all bodies will reflect the same material.

 

QUESTION - When using Model States to display the steps in the process of a casted finished part, will these steps reflect to the BOM as parent-child?

ANSWER – The BOM for each Model States will update to reflect the components in that Model State.

 

QUESTION - What is the work flow for using 'Library' Model State parts? Is it similar to how you would use iParts?

ANSWER – If I understand this question correctly, I think that I am being asked: "When placing a component in an assembly, can you select a specific Model State to be used within a custom library part? I am assuming that this is just a library part outside of Content Center." If so, Yes! When placing the component, go to Options on the 'Place Component' dialog box and you can select the Model State version you want to assemble. If you are referring to custom content center files, I have not tested this but in reading the following AKN article (Model State - Inventor 2022 - Autodesk Community - Inventor) there is mention by Paul Munford of Autodesk that for adding libraries to content center that you will want to continue using iParts. I would suggest asking further questions on the planned workflow to Autodesk on this discussion panel.

 

QUESTION - Is there a way to change text parameters between Model States?

ANSWER – User defined parameters such as text parameter cannot be assigned to a Model State.

 

QUESTION - If you simplify an assembly with Model States, can you keep the link in order to change the simplified part later driven by original assembly?

ANSWER – In testing this it looks like the Model State is simply used as the starting point for the simplification, and no associative link is kept. I was able to modify the simplified model (by right-clicking and select Edit Simplified Assembly) but it generates the simplified assembly again and overwrites the file.

 

QUESTION - If you have an iPart with a Custom entry that creates a 'custom part' in the workspace, would it still be best to continue to use that iPart or can a Model State part be placed as a 'custom' part?

ANSWER – If I understand this question correctly, I think I am being asked: "When placing a component in an assembly, can you select a specific Model State to be used?" If so, Yes! When placing the component, go to Options on the 'Place Component' dialog box and you can select the Model State version you want to assemble.

 

QUESTION - If you have been using iPart standard fittings stored in a Library, then you change them to a Model State part, will you be able to just place that single file instead of it placing a generated member?

ANSWER – Yes, Model States do not generate separate member files so the single file is placed and during placement you specify the Model State version that is assembled. This is done in the 'Place Component' dialog box by clicking 'Options' and selecting the required Model State.

 

QUESTION - Does design assistant work with Model States?

ANSWER – I am not fully sure of what you mean “work with Model States”, but I just opened an assembly in Design Assistant and there is no data inside of the Design Assistant that recognizes that there are Model States in the file. I hope that helps.

 

QUESTION - If you have an iPart with a Custom entry that creates a 'custom part in the workspace, would it still be best to continue to use that iPart or can a Model State part be placed as a 'custom' part?

ANSWER – Yes, I think that you might be right with this. Model States are tied to features, iProperties, materials, components and you can’t add a custom entry. In fact, you can’t even add a User text Parameter and vary that between Model States.

About the Author

Jennifer MacMillan

Manager – Learning Content Development<br><br>Trained in Instructional Design, Jennifer uses her skills to develop instructor-led and web-based training products as well as knowledge profiling tools. Jennifer has achieved the Autodesk Certified Professional certification for Inventor and is also recognized as an Autodesk Certified Instructor (ACI). She enjoys teaching the training courses that she authors and is also very skilled in providing technical support to end-users. Jennifer holds a Bachelor of Engineering Degree as well as a Bachelor of Science in Mathematics from Dalhousie University.

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