Merge 3 Parts Together

[Anonymous]

I have 3 parts, 2 of which I copied as solid bodies, that I am attempting to do a combine feature with to create a "molded" part to fit the end of the two copied parts; however, when I attempt to combine the features, I am getting a failure. I can combine the raw block and one of the copied solids, but not the other. If anyone could offer any sort of guidance on this matter, I would greatly appreciate the help.

[TheCADWhisperer]

Are you familiar with working in the Repair and Construction Environments (I recommend that you install all Service Packs for your version of Inventor)?

I found several issues that should be fixed. 

This is expert level endeavor.

[Anonymous]

I'm not all too familiar with those environments, but I do know how to at least get to the repair bodies page. The two solid bodies that are complex shaped were sent to me by the customer so I didn't check to see if it had any errors. Is there an easy way to fix these bodies in Inventor 2015? That is the current software that I am running.

[TheCADWhisperer]

It occurred to me that you might only need a small portion of the geometry for the purpose of creating tooling.

If that is the case - you might first cut way anything you don't need.

Save as STEP and then bring back the reduced geometry.

I have had more success with the Construction Environment than the Repair Environment.

The Construction Environment is hidden and must be enabled in Application Optiions,

I thought when I checked your iProperties that it stated 2015 SP1

there is a Service Pack 2 with 5 updates.

Make that SP2 with 6 Updates.

[Anonymous]

I'll have to download Service Pack 2 before I can download the updates, correct?

Also, in regards to creating the tooling, I found it strange that I could combine the raw block with either of the solid bodies but could not combine with the second body after that. I will attempt to download the service pack and the following updates and see what I can do with these options.

[Anonymous]

I also attempted to just extrude away a majority of the part that isn't getting "molded" to create the tool. However, when I do this, I'm left with small chunks of the solids that still won't combine with the raw block. I'm not sure what approach to take from here.

[TheCADWhisperer]

I would write those out to STEP.

Read them back in (this will eliminate any reference to the removed material.

Copy to Construction and delete the imported geometry.

Edit Construction and 

Unstitch all

Run Quality Check on the unstitched surfaces.

Repair/replace any surfaces with errors.

Stitch it all back up.

Run Quality Check again.

Promote (Copy Object) back into the Modeling Environment.....

[johnsonshiue]

Hi Tommy,

The two import solids are not in good shape. Do you have the source files? Are they STEP or CAD files from a competitor software? Without seeing the source files to prove, I guess the solids were already bad before being brought to Inventor. Also, the badness isn't isolated. There are just too many places. You could try using Repair Process to fix up the badness. But, you will probably need to remodel quite a few faces and edges. If you have the source files, it will help us to tell how the bodies become bad and we may be able to offer some options.

Many thanks!

[BeKirra]

With the complexity of features that I see, I am wondering if it was better to put them in an assembly.

[WHolzwarth]

I've repaired both bodies with errors in Construction environment (CE), but unfortunately I've used 2017.R4.

A zip with STEP is attached, nice to see that it's only about 9 MB.

Another issue I've noticed: Response times in CE were remarkably long, together with a flickering + sign at cursor position.

I'll check that later today with a new attempt in 2015.

[WHolzwarth]

Response times in 2015 CE were about the same, but repairing still showed errors after copying back to modeling environment.

Importing above STEP to 2015 showed errors. Import to 2016 was clean, same with 2017 and 2018.