Pattern Driven Pattern in Inventor Assembly

[jaskiratVPK8U]

Is there any option for pattern driven pattern in inventor assembly just like in Solidworks?

see video:

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

[blandb · Accepted solution]

You are looking for a feature driven pattern at the assembly level.

If you have a linear or circular pattern, and you place your fastener in the parent hole of the linear or circular pattern of the part. At the assembly, start the pattern command and choose feature driven pattern. Just select the pattern you want the fastener to follow, and it will auto populate the pattern.

Hope that helps

[JDMather · Accepted solution]

In this video I demonstrate how to create a complex Component Pattern (you might want to skip ahead to 10 minute mark).

[jaskiratVPK8U]

thank you

[rcoelho_design]

Hello,

I'm used to SW driven patterns and I'm finding some issues with a similar feature in Inventor. I could use some help, please.

I’m working with two iPart in an assembly, both created using similar methods. However, one displays its features in the browser (Modeling tab), while the other only appears as a single Solid Body (Pattern PNG).

I suppose this is causing issues because I need to apply a pattern of threatened rivets using the component pattern, but I can’t select the feature pattern of the first part of the assembly (the software also doesn't recognize the feature automatically - Pattern_01 PNG). Meanwhile, I could do it in the second part.

I've noticed that the iPart icon is different for each component in the browser, which might indicate different configurations. Both parts were created as iParts from the beginning, and I need to keep them as iParts to manage multiple size variations.

What I need help with:

• Why does one iPart show individual features while the other doesn't?
• How can I ensure that my iPart retains its features so I can apply a pattern of fasteners in the assembly?

Thanks in advance for any insights!

[johnsonshiue]

Hi! If I understand your issue correctly, this has something to do with iPart member file. iParts were designed to create library components like nuts and bolts. 

An iPart member file is a derived part of the iPart factory file. Within the iPart member file, only the body geometry is derived. There are no feature definitions.

In order to drive a component pattern, you may convert the iPart into a Model States part. Here is the process.

1)  Save the iPart factory file as a new file.

2) Edit the table in Excel. Copy the table to a new Excel spreadsheet. Finish edit.

3) Delete the iPart table.

4) Create a non-Primary Model State -> edit the Model State -> copy and paste the iPart table to the Model State table.

5) Lastly, swap out the iPart with the Model States part.

I believe you can select the part feature to drive the component pattern.

Many thanks!

[rcoelho_design]

Thanks @johnsonshiue for your reply.

Well, I did as iPart because I read about it and believed it was the best tool for managing part numbers/stock. But from what I could understand I also can manage that within design states (through individual iproperties). I will give it a try, but I need the specific Part Number to be listed in the tree ad BOM.

For now, I don't have that many configs in iPart table. Is it safe to keep the part deleting the iPart table (jump steps 1 and 2) and make design states instead?

Thanks for your help.

[rcoelho_design]

@johnsonshiue  After my initial post, I realized that when my features are created under the folded model, they don’t appear in the assembly.

All the parts shown in the images were generated using iPart tables, but the one without a folded model (part template) allows me to select the pattern feature for driven fasteners.

1. Could this be related to the difference between part and sheet metal modeling?

2. Is it possible to create a driven pattern for fasteners in an assembly when working with sheet metal parts, or is this functionality limited to standard part templates?

Any insights on this?

Thanks!

[johnsonshiue]

Hi! I don't think the issue is between a sheet metal part and a regular part. The difference is you have a converted iPart factory and an iPart member file in the assembly. The iPart factory (the one with nested table nodes), though, contain the features, it is not meant to exist in an assembly. This is because the factory itself is like an iPart member generator. Its function is to create iPart member files (derived part of the iPart factory).

I guess before the part was converted to an iPart factory, it was just a sheet metal part, consumed by the assembly. Then the sheet metal part was converted to an iPart factory. The next step you should have done is to replace the converted iPart factory with one of its own members.

I just don't see a way that iPart can drive Feature-Based Component Pattern. To drive such component pattern, you need to have the feature definition but an iPart member does not have the feature definition as the iPart factory. The only way to make it work is to use Model States.

Many thanks!

[rcoelho_design]

Hi,

I did it, and it was very smooth with model states.

IPart creates new part files for each member but Model States don't, am I correct?
Is it okay since I can control part numbers, descriptions, stock, BOM, and specific features with this method.

Thank you very much for your help! 

[johnsonshiue]

Hi! Yes, iParts and Model States parts behave very similarly (driven by a table). The major difference is that iParts do generate individual member files, while Model States parts wrap every members in one ipt file.

Though they are similar, I personally would use them for different purposes. iParts are best for library components like nuts and bolts. Their definitions are rarely changed. Model States parts are better for referencing purpose (like your workflow) or showing variations of geometry.

Many thanks!