Workflow for Parts with Multiple Operations

[DavidTunnard]

Hi all,

Some parts that we have manufactured start off as laser-cut blanks and are then some features machined afterwards.

For most parts I can get away with having one part file. However some more recent parts have meant, that to show a distinction between the laser-cutting and machining on the drawing, I am needing to create two part files. One file being the laser cut 'blank' and the other being a derivative showing the machined features.

Ideally I want to only have one part file and one drawing file. Is there anyway of doing this?

Apologies if that doesn't make much sense. I wasn't sure how to word my problem! Please comment if you would like some clarity.

Thanks,

David

[dan_inv09]

So you do derive the laser cut part into a new part to do the machining?

You could put the laser cut part in an assembly and machine there - it's still two files

or then you could make the assembly a weldment and machine in both Preparations and Machining and then you can place views of the finished machining or the prep machining or the just the part(s) before

Without a second part file we can do but I don't think there is a way to do it without a second file.

[mcgyvr]

Derived parts or iparts..

An ipart will allow a single "factory" file to control everything which may meet your needs of a "single part file" even though its really creating multiple files in the background.. 

Either option allows a single drawing file

[johnsonshiue]

Hi David,

At the moment, Inventor part or assembly can only have one geometric definition at any given moment. If you want another geometric definition, you need another part. Like Dan and Brian mentioned here, you can use Derive or iPart to create variations. But, just like I mentioned, it requires multiple parts.

We are working on a project called Alternative Representations, allowing you to create multiple states of the model. If you are interested, please sign up Inventor Beta (https://autode.sk/InventorBeta). You can try it on the latest install-free/browser-based build. Also you can give feedback to the project teams.

Many thanks!

[jtylerbc]

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@DavidTunnard wrote:

Ideally I want to only have one part file and one drawing file. Is there anyway of doing this?

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It's not currently possible to do this with a single part file.  As others have mentioned, the common ways to do this are to either:

1. Use derived parts (2 part files).  Model the blank first, derive it into the second part, then add the machining features.
2. Use a weldment assembly.  Model the blank first, insert it into the assembly, and machine it there.

These are also the common techniques used to model castings that get machined.  There is technically nothing wrong with either method.  But having my "finished part" actually be modeled as an assembly has always felt a little strange to me, so I have always tended to use the first method.  Both result in two files, so there is no difference in that respect.  If you have differing final machined parts that are produced from a common blank, this two-file method is actually beneficial. 

In both cases, you can place views of the blank and finished versions on the same drawing if there is sufficient room, but there still will be two 3D model files.

At my previous employer (where I did most of my cast/machined part work) we had transitioned from another CAD package where we already used an equivalent process to the Derive method.  So we naturally carried that logic over to the most similar technique when we transitioned to Inventor. 

I have also experimented with the weldment machining method a little, but at that same company, this would have been potentially confusing due to the way our part numbering system worked.  So we ended up just sticking with what we knew.

iParts are a method that seem like they could work, but I don't have any experience actually using them that way. They are originally intended to make it easier to model families of related parts.  I find working with them to be cumbersome enough that I tend to only use them for what they're really good at.  

[DavidTunnard]

Thanks to everyone for the replies.

Yes, what we currently do is create a blank and then derive it into another part file. The only problem we have with that is the derived part loses the material properties for some reason and re designating them sometimes gets forgotten about. No big deal though.

[DavidTunnard]

Cool! I will have a look into it and leave some feedback. Thanks for letting me know!

[jtylerbc]

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@DavidTunnard wrote:

The only problem we have with that is the derived part loses the material properties for some reason and re designating them sometimes gets forgotten about. No big deal though.

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Yeah, that can be a problem.  Even as often as we did this operation at my previous job (almost half of our parts were modeled this way), it still got missed occasionally.

It would be nice to have the ability to link the materials through the Derive operation.

[SBix26]

Way late to the party, here, sorry...

There is a technique using a single part file that may do what you want, using multiple solids.

• Create your blank
• Use the Rectangular Pattern tool, checking the Pattern solids option, and select Create new bodies; pattern in one direction, 2 instances, a convenient distance away; this gives you a copy of the original as a separate body
• Add features to the patterned body as needed to define the final form
• Create two view representations, one for each body, with the visibility of the other turned off
• In your drawing(s), use the view representations to control which body is displayed in a particular view

The patterned body is an exact copy of the first body, so any changes to the first body are reflected in the pattern; you can add, alter, or remove features above the Pattern feature, affecting the blank and the finished part; you can add, alter, or remove features below the Pattern feature, affecting only the finished part.

All the work is in one file, that's the advantage.  But the disadvantage is that you actually have two bodies in that file, so you have to keep hiding one of them (using view reps) in assemblies and drawings, and all your physical properties (mass, volume, surface area, etc.) will be wrong.

If the disadvantages aren't serious for your situation, this might work for you.  I use that technique for progressive work, though I typically derive out the individual solids into separate files for detailing.  But it's much easier to edit when all the definitions are in the same file.

Hope this helps,

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Sam B
Inventor Pro 2021 RTM | Windows 10 Home 1903
LinkedIn

[HAFA12]

I use the flat pattern to hold my "laser cut blank" part. Features in the flat pattern will only apply to the flat pattern. So I add my overlength, extra material for machining, fill holes that will be machined etc.

The folded model will hold all the normal features of the machined part.

So use a sheet metal part if it's cut from plate stock..