topic Re: General Questions Regarding Functionality of Iparts and Iassemblies in Inventor Forum

General Questions Regarding Functionality of Iparts and Iassemblies

eric.frissell26WKQ — Thu, 22 Jul 2021 13:33:05 GMT

Hi guys, for starters I am a SolidWorks Professional who's now working in Inventor so approaching the topic of iParts and iAssemblies, the SolidWorks configurations is my frame of reference and generally how I expect workflow to be handled. So in saying that I've built some iParts and iAssemblies to get some understanding of how Inventor handles them so I can implement them in my designs but I do have some questions regarding how the vault handles them or how they're designed to be used within the manufacturing process.

First question is regarding the creation and deletion of iParts and how it's dealt with by the vault. In SolidWorks you could create and delete configurations to your hearts content because configurations are contained within the part. With each iPart member being its own file in the vault how does this differ from above? If you delete an iPart from the table will it automatically be deleted from Vault? What if the person deleting the iPart does not have the ability to delete parts within the vault? Are vault exceptions granted and the part deleted or does the member become disassociated (maybe lose it's link is the better way to say this) to the original part? Anything important to know regarding it handling a change in member names?

Second question is regarding drawings. What is the proper way to handle having an iPart library of manufactured parts forcing you to have multiple drawings? In the drawings I see you're given the option to switch between members in the drawing views so presumably you could have 1 drawing with multiple sheets and each sheet represents a different member. Presumably you could also have each member on a different drawing. We use an automated vault release system through the Item Master that auto creates PDF's so are there any headaches getting an iPart through the automated system? Anything important to know? If there are individual drawings for individual members would the vault release all the members upon the iPart itself being released?

Also regarding drawings I notice the dimensions disappear when you switch between iPart members? If the only change to members is that they increment in length is there a way to keep those dimensions as you switch between members? How do you create your drawings quickly and efficiently if the dimensions disappear when members change?

Are iProperties a global property of the iPart itself rather than iProperties being individual to each member? I.e. the iProperties do not change as you switch between members. Given this what is the proper way to reference a change of material in each member?

In SolidWorks you could also end the SolidWorks calculation of design tables if you skip a row (this was equivalent to the $User_Notes command) so you could essentially have all your parameters go until a certain point and if you skip a row the parameters would quit evaluating. This would allow you to have headers for any calculations/equations and SolidWorks would not evaluate them as a parameter. Will Inventor do roughly the same thing?

Another important SolidWorks tidbit is that it was important to rebuild your configurations so you could find out if something broke (and it would let you know), is there an Inventor equivalent to this? If one of the iPart members break then how does it tell you other than having to click through each individual member?

For anyone who's gone from SolidWorks to Inventor and has used configurations and iParts what were the biggest changes you dealt with? Anything that would be helpful to know?

Thanks

Re: General Questions Regarding Functionality of Iparts and Iassemblies

swalton — Thu, 22 Jul 2021 14:36:53 GMT

iParts and iAssemblies are not a flexible as Solidworks Configurations. The Model States function introduced with Inventor 2022 comes closer.

What version of Inventor are you using?

If you add Vault to iParts and iAssemblies, they get less flexible.

Basically, I plan all the possible variations of a component and add them to the iPart table before I check anything into Vault. Once the iPart factory is in Vault, any edit to it also requires checking-out and updating every member file.

Re: General Questions Regarding Functionality of Iparts and Iassemblies

eric.frissell26WKQ — Fri, 30 Jul 2021 13:11:47 GMT

You pretty much stated my biggest fear with Inventor. Everything works pretty well until something changes and then it all goes to ****.

Currently using 2020. What does the update process look like for updating every member? Checkout and open the iPart factory, check out all members, individually click each configuration and rebuild like Solidworks pre-2017, or is it a litle different?

If a member is deleted or renamed that has been checked into the vault will the vault delete it or update the name or just create a new member and leave the old one dangling around?

Edit: also if you don't mind how do you handle drawings for each variation? You'd assume with the way the vault operates each member needs a drawing.

Re: General Questions Regarding Functionality of Iparts and Iassemblies

A.Acheson — Thu, 22 Jul 2021 15:12:32 GMT

“Second question is regarding drawings. What is the proper way to handle having an iPart library of manufactured parts forcing you to have multiple drawings? In the drawings I see you're given the option to switch between members in the drawing views so presumably you could have 1 drawing with multiple sheets and each sheet represents a different member.”

I don’t normally document individual members but simplify place one member and use the ipart table to show the variations and add extra columns for parameter variations say length for change in length. For iAssembly you can switch the parts list per member also.

If you want to automate ipart/iAssembly drawings you can simplify detail one drawing and do a save as and then replace model reference to replace member. Then you can automate this with ilogic which is very effective.

“Also regarding drawings I notice the dimensions disappear when you switch between iPart members? If the only change to members is that they increment in length is there a way to keep those dimensions as you switch between members? How do you create your drawings quickly and efficiently if the dimensions disappear when members change?”

For the most part they should remain but if there is drastic change in size they will disconnect. I have notice they move about quite alot because the stand off distance is not fixed they can end up over geometry or in completely the wrong position. Hole and radius dimensions can be very unpredictable.

“Are iProperties a global property of the iPart itself rather than iProperties being individual to each member?”

iProperties are independent for each member. If you want independent properties per member add it to the ipart table.

“Another important SolidWorks tidbit is that it was important to rebuild your configurations so you could find out if something broke”

I don’t think there is any built in functionality for this. You could use some ilogic rule to check for errors by looping through all the members.

Saving or clicking on the member is necessary to commit any change done through an iLogic form or iLogic and a rebuild all using the command button and generate member can be necessary to update iParts/iassemblies to there members. They are a bit hap hazard in this regard leading to frustrations if your using them daily.

Re: General Questions Regarding Functionality of Iparts and Iassemblies

eric.frissell26WKQ — Thu, 22 Jul 2021 18:18:23 GMT

Thanks Acheson, this helps clarify a few things. In our case we need individual drawings because they contain flat patterns which need to be exported as DXF's, which I've found the drawing creation/update process to be pretty simple. Dimensions being deleted from one member but reappearing when you revert back to the dimensioned member was a result of the "Preserve Orphaned Annotations" not being checked. Presumably that would allow you to make individualized annotations on each member, set the drawing views to "Active Member", and utilize 1 drawing for your iPart factory. An egregious abuse of best practices IMO but someone has probably found it useful. Haven't made an iLogic rule for drawings yet but to be honest what one would go through to create one looks pretty simple.

Any chance you've worked with the Item Master and assigning iPart members to items? All our components require a drawing but it appears assigning an item to one of the iPart members now wants to take EVERY drawing with it. This will be confusing

Re: General Questions Regarding Functionality of Iparts and Iassemblies

johnsonshiue — Thu, 22 Jul 2021 20:14:24 GMT

Hi Eric,

Let me quote your posting so I can embed my reply.

@eric.frissell26WKQ wrote:

Hi guys, for starters I am a SolidWorks Professional who's now working in Inventor so approaching the topic of iParts and iAssemblies, the SolidWorks configurations is my frame of reference and generally how I expect workflow to be handled. So in saying that I've built some iParts and iAssemblies to get some understanding of how Inventor handles them so I can implement them in my designs but I do have some questions regarding how the vault handles them or how they're designed to be used within the manufacturing process.

[JS]: I know a thing or two about SWX. I have to say INV iPart/iAssembly is not SWX Config. At least it is not an equivalent workflow. If you were told otherwise, the person was misinformed. INV iPart/iAssembly was meant to create library components like nuts and bolts with similar shape but different sizes. Each iPart/iAssembly member is a distinct file driven by its factory file. The best approach to handle iPart/iAssembly in Vault is to author, elaborate, and lock up. Library components should not change constantly.

First question is regarding the creation and deletion of iParts and how it's dealt with by the vault. In SolidWorks you could create and delete configurations to your hearts content because configurations are contained within the part. With each iPart member being its own file in the vault how does this differ from above? If you delete an iPart from the table will it automatically be deleted from Vault? What if the person deleting the iPart does not have the ability to delete parts within the vault? Are vault exceptions granted and the part deleted or does the member become disassociated (maybe lose it's link is the better way to say this) to the original part? Anything important to know regarding it handling a change in member names?

[JS]: I think my reply above pretty much captured the question here.

Second question is regarding drawings. What is the proper way to handle having an iPart library of manufactured parts forcing you to have multiple drawings? In the drawings I see you're given the option to switch between members in the drawing views so presumably you could have 1 drawing with multiple sheets and each sheet represents a different member. Presumably you could also have each member on a different drawing. We use an automated vault release system through the Item Master that auto creates PDF's so are there any headaches getting an iPart through the automated system? Anything important to know? If there are individual drawings for individual members would the vault release all the members upon the iPart itself being released?

Also regarding drawings I notice the dimensions disappear when you switch between iPart members? If the only change to members is that they increment in length is there a way to keep those dimensions as you switch between members? How do you create your drawings quickly and efficiently if the dimensions disappear when members change?

[JS]: In terms of drawings, to certain degree, iPart/iAssembly is not much different than a regular part/assembly. They are distinct files. However, model dimensions cannot be retrieved because the iPart/iAssembly members are different files than the factory files. The actual dimensions reside in the factory files, not the member files. Also, after you annotate drawing view based on an iPart/iAssembly member, you cannot easily change the model reference to a different member. The annotations will become sick or gone. It is as if the source files have been swapped. Typically, the iPart/iAssembly is documented in one variation. Then the configuration table is attached to sheet showing all the variants.

2022 Model States is more similar to SWX Config, since it wraps all variations within the same file. So, the above iPart/iAssembly drawing behaviors do not happen to Model States.

Are iProperties a global property of the iPart itself rather than iProperties being individual to each member? I.e. the iProperties do not change as you switch between members. Given this what is the proper way to reference a change of material in each member?

[JS]: iProperties in iPart/iAssembly/Model States are all member-based. Each member can have a different set of iProperties values.

In SolidWorks you could also end the SolidWorks calculation of design tables if you skip a row (this was equivalent to the $User_Notes command) so you could essentially have all your parameters go until a certain point and if you skip a row the parameters would quit evaluating. This would allow you to have headers for any calculations/equations and SolidWorks would not evaluate them as a parameter. Will Inventor do roughly the same thing?

[JS]: I believe if you do that in Inventor, all the rows after will be invalid.

Another important SolidWorks tidbit is that it was important to rebuild your configurations so you could find out if something broke (and it would let you know), is there an Inventor equivalent to this? If one of the iPart members break then how does it tell you other than having to click through each individual member?

[JS]: In INV, you will have to enable a member in order to see how it behaves. Rebuild All can recompute a given member. Generate files (iPart/iAssembly) can help create the members. If there is something wrong, you will see an error. But, it does not apply to Model States.

For anyone who's gone from SolidWorks to Inventor and has used configurations and iParts what were the biggest changes you dealt with? Anything that would be helpful to know?

Thanks

Many thanks!

Re: General Questions Regarding Functionality of Iparts and Iassemblies

A.Acheson — Fri, 23 Jul 2021 00:46:08 GMT

I cannot answer to vault questions unfortunately. Below is some ilogic codes to save as drawings for iParts/iAssemblies.

Here is a code in the link below and the last post for creating iAssembly members to drawing.
If you detail the first member up and include all notes save then run the rule. You will notice some annotations move around as the member views increase etc. But hopefully they are only simple tweaks required.

For iParts view the post here message 12 of 20. Simply remove the word set to convert to ilogic.

Re: General Questions Regarding Functionality of Iparts and Iassemblies

eric.frissell26WKQ — Fri, 23 Jul 2021 12:45:26 GMT

Thanks for the reply Johnson, just looked into Model States and without digging too deep it looks like they're a middle ground between SolidWorks Display States and Configurations. This is great because they are two things that I've really missed along with how simple it was to use them. Regarding the Model States it would be alright to have multiple 'configurations' of sheet metal parts, right? And you'd be able to generate individual drawings per model state enabling you to have a flat pattern / DXF per model state?

Re: General Questions Regarding Functionality of Iparts and Iassemblies

johnsonshiue — Fri, 23 Jul 2021 23:27:35 GMT

Hi Eric,

The answer to your both questions is yes and yes. Model States addresses the particular request you are asking. But, it still not 100% equivalent to SWX Config.

1) Model States does not allow you to suppress an occurrence (across multiple levels). You will need to suppress the instance within the subassembly.

2) Skeletal modeling and adaptivity are not fully supported in Model States.

Many thanks!

Re: General Questions Regarding Functionality of Iparts and Iassemblies

eric.frissell26WKQ — Wed, 28 Jul 2021 12:13:13 GMT

Thanks for the heads up, but mind if I ask what the difference between an occurrence and an instance is, and if that is regarding a part feature or perhaps an assembly item?

Re: General Questions Regarding Functionality of Iparts and Iassemblies

johnsonshiue — Wed, 28 Jul 2021 20:18:59 GMT

Hi Eric,

Yes, this is very insightful question. From Inventor's perspective, there is a difference between instances and occurrences. So, instances mean the components are at the same level. Let's say, you have an assembly with two Part1 (two identical parts). These two are instances.

Occurrences mean the components are at different levels. For example, you have an assembly with two Part1. But, one is right within the top-level, but the other one is within a subassembly.

Inventor Model States can only control things happening within the same level, not across levels. I was told that SWX sort of "supports" cross-level suppression. I am not a SWX expert to confirm it for sure.

Many thanks!

Re: General Questions Regarding Functionality of Iparts and Iassemblies

CGBenner — Fri, 30 Jul 2021 13:13:18 GMT

@eric.frissell26WKQ Did the information provided answer your question? If so, please use Accept Solution so that others may find this in the future. Thank you very much!