Cavity of a surface part
I've attached test parts and an assembly of how I would want the surface part nested in the nest block. I also attached a screenshot of the tree of the customers part showing the warning. Not sure if this might be part of my issue.
Hi! I am sorry I am a bit confused here. I am able to derive the assembly to a part without an issue. What is the workflow leading to the failure?
Many thanks!
@landin.griffin wrote:
... the customers part showing the warning. Not sure if this might be part of my issue.
I would want to clear this issue first.
Right click on that body and select Repair Bodies.
Then select Find Errors
Click Select All
OK
You should now have a green checkmark next to the body, click Finish Repair.
If you do not have the green checkmark - then the repair is going to take expert level experience and it will be necessary to have the actual file. If it is proprietary then @johnsonshiue can check under non-disclosure, otherwise Attach it here.
For what you want to do - I don't think you really need an assembly.
You might not even need a separate part.
There are three ways to do this.
1. Within a single part.
2. Derive the surface body into a new part and build the nest using the surface body.
3. Derive the surface body and the nest assembly into a new part....
I don't think these can be adequately demonstrated with the dummy files that you attached as I don't think that they accurately replicate the true issue that you are experiencing with your customer file.
I repaired the body and got the green checkmark and tried to derive the assembly with the nesting block where I want it on the customers part into a new part subtracting the customers part and the result looks like this. It didn't remove the customers part.
I tried doing the same method with the test assembly I attached and got similar results. So it looks like we tracked down the issue, my ignorance haha. I personally don't know how to achieve creating the negative other than the method I've described. You stated two other methods but, I don't understand how to go about doing them.
@landin.griffin wrote:
I want it on the customers part into a new part subtracting the customers part...
How are you doing a "subtract"?
Below is the method I tried.
I also just tried sculpt with the test parts and the customers parts and got did not produce meaningful results with each.
For Sculpt my work flow is as follows:
I opened the assembly with the surface and solid part.
I opened the solid part inside the assembly.
I used Copy Object to pull the surface into the part.
I then used Sculpt, selected the surface and chose remove.
Hit okay and I get the "did not produce meaningful results" error.
Hi! In Derive Assembly, only the solid bodies get Boolean. The surface bodies do not participate. In your case, you have one solid body part and one surface body part. They won't cut in the Derive process. You can simply include all the bodies. Then use Sculpt or Split command to cut the solid body with the surface body.
Many thanks!
Thank you for the information on derive, I did not know that. I am however still having issues with sculpt and split. I can't seem to get either of them to work with the test parts. Below I've attached some snapshots of my work flow and hopefully you can see where I'm going wrong, thanks in advance for any insight you may have. I also realized I never said what year inventor I'm using, I'm in Professional 2021.
Open Test Assembly and the parts are constrained where I want them.
Open the Nest Block inside the assembly and use copy object to pull in surface body. (I've tried composite and surface)
Start a sculpt and select composite and remove. (I've tried changing the direction of sculpt with same results.)
Click okay and this is may result.
It should work using Sculpt. How about attaching your test assembly and two files here so someone else can see what's wrong.
But this would be easier using Derive: derive the "cutting part" into the nest part as a solid body; use Direct Edit > Move body (or Move Body tool) to reposition, if necessary; Combine/cut; clean up entry passages, lead-ins, etc.
Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn
Hi! Please edit the Sculpt and change the surface direction. It is possible it tried to cut both sides. Please attach the files here if it still does not work.
Many thanks!
Here's a part derived from the Test Assembly, and then sculpted to make the nest. But this was a lot more difficult than it needed to be because of the part constructed of surfaces instead of a solid.
It would be much simpler to work with a solid in this case, allowing the Combine tool to be used with two picks.
Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn
Hi! I took a look at the files. I think I know where the problem is. The issue is with the surface part. There is a redundant boundary patch surface, which creates a non-manifold body. Simply hide it and trim off the top surface. It will work better.
There are actually two solutions here: Copy Object (adaptive body) vs Derive. Please take a look at attached files.
Many thanks!
