Top Down Modelling with Configurations

[JEA2022]

I'm new-ish to Inventor and have been struggling to do decent Top-Down design in a way that makes mass producing drawings with lots of different configurations quick and efficient.

What I want 

1. Have a top level something that I can draw all my parts in together and define in system wide parameters that do not change per configuration (eg wall thickness if everything is from the same material)
2. Have individual part/assembly files that I can designate which configuration (A, B, C, D in the image below) I want use Model States/iPart/iAssembly  
3. Have drawings for each ipt/iam with multiple sheets showing identical dimensioning for each configuration (eg Config A goes on S1- Sheet 1, B to S2)

 I have watched a lot of videos (1 ,2,3,4,5) and read a few Top-Down design guides (6,7 ,8 )  but have thus far been unsuccessful in finding an effective way of doing what I want. This answer given by @BDCollett here seems to indicate that it is possible to do exactly what I want to be able to do for Attempt 2 below, but I haven't been able to do so. Other answers (eg this by @CCarreiras ) seem to indicate that this kind of task is better suited to iLogic, however as you will see below I have had issues where iLogic works fine in parts/assemblies but trying to get dwgs to show the right geometry does not work. If anyone has any ideas/tips pointers I would greatly appreciate it.

Attempt 1: Skeleton Modelling
This is the method I still use as it is the fastest, however it still requires a lot of repetitive tasks that are time consuming and very inefficient. Issues are:

• Use of iLogic to pass parameters from Master Assy to Master Part does not seem to be the intended purpose, as although the Assy performs as expected, the geometry does not change in drawings using configurations  
• This method does not involve individual part configurations (whether by iPart or Model State) as to update the geometry shown on the drawings, the underlying model configuration must be manually changed, meaning it is much faster to just change the assembly file (instead of each individual part file).

 

 

Attempt 2: Multi-Body Modelling
This method is so close to working but fails because I cannot programmatically edit from which configuration a Derived Feature comes from (in my image below I show that this can be done via iLogic but as with above, this does not translate to being able to update the geometry on the drawings).
Additional issues include:

• If any of my sub parts are sheet metal parts I have to make my Master Part a sheet metal part, ruling out the us of Rule Fillet and other useful tools
• Because I cannot choose the Model State/ iPart representation of a derived solid I have to create a full set of ipt files for each configuration. I am sure this could be automated using iLogic 
• However, when creating drawings I want each sheet to be essentially identical (same views, same sections, same dimension locations), however as the "Component File" of a drawing view cannot be changed after placement this means that I have to recreate every sheet from scratch which is significantly more time consuming that my Skeleton Modelling Attempt

 

[swalton]

I don't do much top-down or skeletal modeling...

Have you used the Replace Reference Model command in the drawing environment to switch out the model in a drawing view?  I find that can be helpful if the models are related and have similar edges/faces/features.  There is still some manual work, but it can cut down on the tedium.  I'm not sure how well it works if you are swapping out different derived parts. See: https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-FC081D92-92AB-4DE0-97B0-72DE7637FAD9

Have you looked at the drawing automation tools like Sheet Formats combined with 3d annotations? 

See: https://blogs.autodesk.com/inventor/whats-new-2022-drawing-automation/

Finally, are you leveraging Design Assistant, iLogic Copy Design or Vault Copy Design to copy previous projects, drawing and all, to support new designs?

[JEA2022]

Thanks @swalton, great tips but unfortunately still doesn't solve the issue with having to repeatedly do essentially the same thing.

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@swalton wrote:

Replace Reference Model

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This wouldn't help for my Attempt 1 as the files are being referenced correctly, just they all provide the same geometry

I didn't use this in my Attempt 2 as when you copy a sheet, it still has the same model reference as the prior. I suppose I could copy the whole drawing and have a separate 1 Sheet drawing for each configuration however this would require more of the manual repetitive work I am trying to avoid. 

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@swalton wrote:

Sheet Formats combined with 3d annotations

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I had not realised what a useful tool this is! I will use this going forward, however for both of my Attempts this still doesn't solve the issue with having to recursively update iam/itp files to display the correct Representation.

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@swalton wrote:

Design Assistant, iLogic Copy Design or Vault Copy Design

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I am not using these design copy tools as I wish the configuration designs to be editable after the fact, so if the supplier comes back and says a detail needs to be changed I can just edit it in the Master model and that will flow on to the rest, instead of having to either model recursively in each copied part or copy all the configurations again and redo all the changes I would have had to have made (scales on drawings, properties etc) 

[A.Acheson]

It seems in both your techniques you need ilogic to automate a few of the manual tasks. Can you list where this is failing? If you can do it manually you can do it by code unless there is a blind spot in the API exposure. 

[swalton]

I don't really follow your workflow.  Like I said, I don't do much top-down design.  

I had assumed that each individual real-world part and assembly was represented by a unique ipt or iam file.  In that workflow, changing the part/assembly file reference would change the geometry shown in the drawing without editing the views.  The concern would be ensuring that the drawing dimension entities connect to the correct geometry when the reference file changed.  In addition, I normally document one and only one model in a single idw file.

It seems to me that Inventor needs some help to understand which model should be shown in which view in a drawing.  An iLogic form or similar might be a way to specify what you want to show.

You might check out some of the Autodesk App Exchange offerings.

Creates drawing views of assembly components

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=6055662968820286099&appLang=en&os=Win64

A way to print a drawing set from individual drawing files

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=3826146264845665861&appLang=en&os=Win64

[JEA2022]

@A.Acheson  :
I have made another post on the iLogic forum, essentially the issue is that the views shown on drawings do not obey the Model State Representation (or iPart/iAssy Member) that I have used iLogic to make manually work in the Part/Assembly environment. If you had ideas on how to make this work then you would completely solve my problem and would have my eternal gratitude.

@swalton 

• changing the part/assembly file reference would change the geometry shown in the drawing without editing the views
  
  • My issue is that this is not occurring for either method, I think due to the iLogic I have used. I would have thought this would work also 
• An iLogic form or similar might be a way to specify what you want to show.
  • I have tried a few different scripts to get the drawings to read geometry from the selected representation instead of the one present in the file, however I have not been successful. I will keep trying but I made this post as I have thus far had no luck.
• You might check out some of the Autodesk App Exchange offerings.
  • I had never used these before, I will give the free one a go and look into other useful apps! Really appreciate all the help you have given me

[CCarreiras]

Hi!

iPart and model states are different things: iPart members are independent files (childs connected to father). Model states, you don't have external files, all states are represented in one file.

[CCarreiras]

It's an assembly with parts with several configurations (model states), right?

I would use just an assembly made of parts with model states.
No derive parts, no assembly, no parts. (why use it?)

Using an iLogic form i would order the parts configuration, from the assembly to the parts.

[JEA2022]

• iPart and model states are different things: iPart members are independent files (childs connected to father). Model states, you don't have external files, all states are represented in one file.

Apologies if my post above is a bit unclear, I included both to indicate I had tried using both methodologies and neither Model states nor iParts could resolve the drawing

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@CCarreiras wrote:

It's an assembly with parts with several configurations (model states), right?

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This is what I want to do, but with the addition of a Master Model, so that I can store all my parameters in one place and dont have to go to each part file to remodel the same feature if I need to make changes. 

• My Attempt 2 above does exactly what you suggest, however the individual part files do not update in Assemblies/Drawings as:
  • Each sub part is a derived solid from multi body Master Part file (this file has all Mode States)
  • In order to create the same Mode States for each sub part I run this iLogic (it changes the Model State of the Master Part from which each sub part is derived)

Option Explicit on
    Dim oDoc As PartDocument
    oDoc = ThisDoc.Document
    
    Dim oDef As PartComponentDefinition
    oDef = oDoc.ComponentDefinition
    
    Dim oDeriveDef As DerivedPartDefinition
    oDeriveDef = oDef.ReferenceComponents.DerivedPartComponents(1).Definition
    
    oDeriveDef.ActiveModelState = oDef.ModelStates.ActiveModelState.Name
 
    oDef.ReferenceComponents.DerivedPartComponents(1).Definition = oDeriveDef​

• This works fine in the Part and updates the geometry as expected, but when placed into a Drawing or an Assembly the part no longer updates and just remains whatever Model State was last selected
• If I put the Master Part into a drawing/assembly then it updates fine

If you have more ideas (beyond those I mentioned in my first post) about how I can do Top Down modelling whilst being able to do configurations please let me know. Appreciate your time.

[swalton]

Do you have a dummy example that you can post?  

I'd like to take a look at it and see your workflow.  I am very curious about the non-updating drawing files.  

[JEA2022]

Please note that I am not super attached to this workflow, I just want to be able to efficiently do Top Down modelling with configurations so posted this query to the forum to see if anyone has better methodologies as I am fairly new to inventor.

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@swalton wrote:

Do you have a dummy example that you can post?  

---

That being said, my current workflow is close to working (failures outlined below), I have attached a zip file of a small project that I have used Pack and Go on.

Each sub-part (bar, plate, rod) has been derived from the MASTER part, and then they have been put into the MASTER assembly.

What works:

• The Model States in the MASTER part
  • If i change the Model State, this changes the parameters and updates the model
    
• The Model States in the sub-parts
  • 
    Using iLogic, if I update the subpart Model State then the part will update to the selected representation

Option Explicit on
    Dim oDoc As PartDocument
    oDoc = ThisDoc.Document
    
    Dim oDef As PartComponentDefinition
    oDef = oDoc.ComponentDefinition
    
    Dim oDeriveDef As DerivedPartDefinition
    oDeriveDef = oDef.ReferenceComponents.DerivedPartComponents(1).Definition
    
    oDeriveDef.ActiveModelState = oDef.ModelStates.ActiveModelState.Name
 
    oDef.ReferenceComponents.DerivedPartComponents(1).Definition = oDeriveDef​

What doesn't work:

• The Model States in the Assembly
  • if i change the Model State, the representation will change but the actual geometry will not
    
• The Model States in the Drawing
  • if i change the Model State, the representation will change but the actual geometry will not 

[johnsonshiue]

Hi! Let me try to answer this question briefly. I don't think Model States or iPart/iAssembly is compatible with any cross-level dependency workflow. Their definitions should be strictly on the table or outside of the table within the component (applying to all members). If you try using one Model State to drive another component, such relationship will only exist in the Model State, not applicable to other Model States.

Many thanks!

[JEA2022]

Does that mean that it is impossible to have a Top-Down workflow with Configurations?
This only requires 2 things:

• Configurable master file containing all sketches/parameters for the design
  • The solids can be modelled in too but dont have to be
• Sub-part files containing all the solids (but no other design info) where I can choose which configuration of the part I want to display
  • Changes to design would only need edits to the master file and these sub-parts would update individually via parameters/derivation

All the sources I have found (1 ,2,3,4,5,6,7 ,8 ) do not give any indication that this is possible, so if this is the case I would be very interested in any workflows that allow Configurable top down design.

[swalton]

Jallchin,

Thanks for posting your sample file.  I'll try to take at look at it tonight/tomorrow at home.  

When I have created very simple top-down designs, I have limited the model to creating a single real-world configuration at a time.  When I wanted to manufacture variations, I copied the design as a unit to new files and then modified the driving parameters in the new master model. 

I've never tried to make a top-down design driven from a master part that several different real-world configurations at a single time.  Based on @johnsonshiue's post in this thread, I am not sure that Inventor supports such a workflow.  iLogic may be able to get the result you want, but I am out of my depth with that tool.  Is there an iLogic command to specify a model state of a drawing view?  

[BDCollett]

Copy Design of an iLogic Assembly driving a Master Part is going to be far less painful than this.

Yes you will have to have multiple files for each configuration of parts, but it's easy to manage.

[JEA2022]

Thanks a ton, I need to a lot of work like this with a fair few configurations so if you had any suggestions on a workflow that would be able to do it all then that'd be appreciated.

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@swalton wrote:

Is there an iLogic command to specify a model state of a drawing view?  

---

This is the method from the API help for setting the modelstate of the drawing view. 

I did try to incorporate it into my workflow but I couldn't get it to work (likely due to my inexperience with iLogic)

Syntax

DrawingView.SetActiveModelState( ModelState As String, [UpdatePartsList] As Boolean, [KeepOverrides] As Boolean )

[JEA2022]

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@BDCollett wrote:

Copy Design of an iLogic Assembly driving a Master Part

So this would be similar to my Attempt 1 workflow in that I would

• Define "configuration" parameters in a master assembly
• Pass these (via iLogic) to a master part file that has
  • no configurations
  • all the parameters/sketches
• For the sub-parts either
  • Derive the sketches into separate ipt files and model the solids
  • Model all in the Main ipt and use "Make Components" to separate into separate ipt files
• Place all individual parts in Main Assy
• Produce drawings of all parts/assemblies required

@BDCollett  your suggestion is to then 

• Use iLogic Design copy to make new sets of all the above files for each configuration
• Go into each configuration's drawing files and edit them to include relevant notes, scaling etc
• If changes are made affecting all configurations then just edit one of these sets of files and delete the rest, then use iLogic Design Copy and re-edit all the drawing files

If this is the only way to do this in IV then I will do it this way, but I feel like if I can manually update the configurations to get the desired result then I should be able to do it using API/iLogic?
Maybe I dont have a thorough enough understanding of the capabilities of iLogic but if you have any other suggestions that can avoid having to recursively make edits I would appreciate your insight.

[BDCollett · Accepted solution]

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@JEA2022 wrote:

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@BDCollett wrote:

Copy Design of an iLogic Assembly driving a Master Part

So this would be similar to my Attempt 1 workflow in that I would

• Define "configuration" parameters in a master assembly
• Pass these (via iLogic) to a master part file that has
  • no configurations
  • all the parameters/sketches
• For the sub-parts either
  • Derive the sketches into separate ipt files and model the solids
  • Model all in the Main ipt and use "Make Components" to separate into separate ipt files
• Place all individual parts in Main Assy
• Produce drawings of all parts/assemblies required

@BDCollett  your suggestion is to then 

• Use iLogic Design copy to make new sets of all the above files for each configuration
• Go into each configuration's drawing files and edit them to include relevant notes, scaling etc
• If changes are made affecting all configurations then just edit one of these sets of files and delete the rest, then use iLogic Design Copy and re-edit all the drawing files

If this is the only way to do this in IV then I will do it this way, but I feel like if I can manually update the configurations to get the desired result then I should be able to do it using API/iLogic?
Maybe I dont have a thorough enough understanding of the capabilities of iLogic but if you have any other suggestions that can avoid having to recursively make edits I would appreciate your insight.

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This is it basically.

If you have some parameters that you know will need to change that may affect ALL your configurations, then you could always either have one master skeletal part with parameters/sketches that you just RE-USE when doing a copy design. Then all configurations will always share these even when changed.

Other option would be to link to an Excel Spreadsheet that again has parameters that are shared globally with all the different configurations.

This is a method I have used.

[johnsonshiue]

Hi! That is correct. Each unique component in Inventor is a separate file (ipt or iam). Model States are document specific and driven by the model state table within the file. The table cannot dictate or manage any cross-document relationship.

As other experts suggested, I believe iLogic + iLogic Design Copy (or Place iLogic Component) will be your solution. However, you will need to manage many files, since each unique configuration needs a new set of files (some can be shared).

Many thanks!

[tomasz.sztejka · Accepted solution]

My attempt to switching configuration was rather complex and only partially successful. Certainly not stable, but time flows, maybe new version of Inventor is better in that manner.

I did create a code which copied f(x) params from spreadsheet to each file in a project. Sounds simple, but is not, since correct parameter must get to correct part, regardless where it is used in assembly tree. Linking parameters will not work due to restrictions put on it by Inventor (boolean, text, spreadsheet layout etc.).

Then I wrote a code which was able to deduce the "who depends on me?" tree, order parts "bottom up" and run copying and updating code on each file in order of appearance.

The stoppers were:

 1. Dealing with multiple occurrences of same part in different configurations. Impossible due to lack of "overlay parameters" concept in internal Inventor design. Model state suggests that it does exist now, at least internally, but I have not played with it.

 2. Inability to "suppress" part in assembly without creating wobbly, hidden "Level Of Detail" which needs to be referenced later in upper level assemblies  and etc for suppression to work at all assembly and drawing levels. Notice without a dedicated iLogic there is no GUI to set "conditional suppression" in assembly while it is in part.

Notice, at the time I tested it part which was suppressed DID appear in BOM. I could not figure out a reliable method to remove it from BOM.

 3. iParts and iAssemblies are absolutely no go. Too messy to deal with them and with configuration.

 4. The whole project is "switched" to specified configuration and any previous configuration is lost. One needs either to copy project for each configuration, what is a pain in where the sun doesn't shine when one needs to keep an archive and provide updates to base project, or export it in "frozen" format (dwf, pdf, stp etc.) to an archive. Vault is practically killed by it.

 5. As usual in Inventor, if change is significant update of part or assembly may produce peculiar result.

 6. Maintenance of iLogic is a pain since, opposite to VBA, it can't link to "per application" code. If iLogic is used in 1000 of documents to do the same job and You need to change the iLogic code, then You need to change it in 1000 documents. Or at least I am too dumb to figure out how could it be done otherwise.

My final result was: Inventor cannot efficiently support configurations. It can be forced in very simple cases (iParts/iAssemblies) but in generic - no.