Break a Derived Link but Maintain Ability to Edit Source Object

[Anonymous]

I’m using Inventor 2013. Currently I have 2 models – part1 is turning details and part2 derives the part1 model and then has further machining details. I need to combine these files as one editable model without external links. Is it possible to copy across all the features from part1 to part2 with the derived command but break the link completely? I know you can break the link however part1 then becomes uneditable.

Thanks very much

[Marco.Takx]

The think the best way for you is to create a multi-body Part.

Make 2 view representations.

[Anonymous]

There are many different ways to achieve this, but how I used to handle this was:

Step 1: Create the raw material as an IPT (blank cylinder in your case)(purchased in my case)

Step 2: Create a Weldment IAM

Step 3: Insert raw IPT into Weldment IAM

Step 4: Do all welding and machining here

Step 5: Create IDW and insert Weldment IAM. You can now show ALL steps into getting to finished product with 1 IAM file. You will also be able to have a BOM/Parts List showing the RAW material (purchased in my case)

The IPT file should not change unless your RAW material changes from the vendor.

I used to make a drawing of this RAW, but it was a STD for purchasing only.

[SBix26]

Adding on to what @Marco.Takx wrote, I would pattern your base part (turning details) a convenient distance away in the same file, making sure to select the New Solid button.  Then add the further machining details to your second solid.  All is in one file, but changes made before the Pattern feature affect both solids, changes after the Pattern feature to the machining details affect only that solid.  Then use View Representations to show them individually in a drawing.

This can also be extended to a third, fourth, etc. pattern to show as many stages in the fabrication process as you wish.

Here's what my test part and browser look like, with the (2016) part attached.

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[WHolzwarth]

At first glance this looked like a good idea to me, Sam.

But aren't there problems with mass properties and placing this part in an IAM?

Walter

[SBix26]

You're correct, Walter.  This works well for design and documentation, but you still need to derive one of the solids (presumably the last one) into a separate part for assembly purposes.  I'm not clear why @Anonymous (the OP) refuses to use linked parts-- seems to be deliberately removing a very powerful tool from their toolbox.

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[Anonymous]

Thanks very much for your suggestions guys. These are some great ideas for creating new parts for manufacture. I really should have given more info in my original post that would have clarified why I can’t use the derive function.

Currently in the company I work for we have about 500 + existing drawings which use part 1 as the turning details and part 2 as the machining details (derived from the part 1 turning details) which are displayed on sheet 1 and sheet 2 of the idw. We’re currently moving to a new ERP system where the drawing files will be linked in to the ERP objects and this system only recognises the finished ipt. and linked idw. as the object which will be manufactured.

As I try to migrate the ipt’s that use derived files it tries to create 2 ERP objects rather than 1 because it’s referencing 2 ipt. files.

That’s why I was wondering in my original question if there’s a way you can essentially change all the exported data from part 1 (to including sketches and features) into the part 2 model and then break the link, so part 2 model is the full editable part with no external references to part 1? Or if there’s any other quick way to combine these 2 parts into 1 but ensuring the end part is fully editable?

Thanks very much.  I really appreciate everyone's input.

Vicky

[SBix26]

So... you've got an ERP system that doesn't know how to work with Inventor, and you're being seriously handicapped in how you can use Inventor.  I sure hope the ERP system offers huge benefits in other ways; if not, it was a really bad choice!

Sam B

[blair]

Most ERP systems are fairly rigid in their structure. We use Syspro and it requires a bit on thought to get both Syspro and Inventor to work.

Sounds like iParts might work. I had a great PDF file that I had posted a couple of times for this sort of work flow but unfortunately just before Christmas I dropped my USB drive and crashed the drive in it. There are copies of it posted on the Forum, you just need search.

It was from an AU 2014 class.

It allows you to take your finished part, convert it into an iPart and than have steps back for all the machining steps back to the raw casting/blank.