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Creating Nest for Part

12 REPLIES 12
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Message 1 of 13
crev64
1039 Views, 12 Replies

Creating Nest for Part

I have tried to ask this questions before and couldn't seem to get anything that would work for me. I have some parts that I need to make a nest for. I get the part from a customer and it's not in the most usable shape. It's just a bunch of surfaces. I can't change anything from it. I create a square block and place both the block and the part into an assembly. In the assembly I place the part in the block how I would like it to go. From there I create my whole mechanism around these nested parts. What I need to do is cut the shape of the part into the block so that I can bring the block into a CNC program and mill it. Can anyone help me find a way to do this?

Crev64
Autodesk Inventor 2015
12 REPLIES 12
Message 2 of 13
jletcher
in reply to: crev64

Use derived component Start a part finish the sketch click derived component find your assembly and subtract the part from the block...

 

 

Message 3 of 13
Curtis_Waguespack
in reply to: crev64

Hi crev64,

 

You can use the Copy Object tool to do this:

http://inventortrenches.blogspot.com/2011/03/find-interference-and-add-tolerance-to.html

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 4 of 13
crev64
in reply to: jletcher

The derived component method looks like its going to work but I can't figure how to get it to do it. I bring the assemby into a part as a derived component. The dialogue box comes up and I choose "Includes the selected part" for the block and "Subtracts the selected part" for the part but it doesnt do anything. Any help?

Crev64
Autodesk Inventor 2015
Message 5 of 13
crev64
in reply to: Curtis_Waguespack

I tried using the interference and scuplt tool. I followed along but when it was time to use the sculpt tool it always came up with the same error "Operation has no effect on part". Its like the program just doesn't see this part at all.

Crev64
Autodesk Inventor 2015
Message 6 of 13
japike
in reply to: crev64

Can you post your part files?

Peace,
Jeff
Inventor 2022
Message 7 of 13
crev64
in reply to: japike

Here are both the part and the block. 

Crev64
Autodesk Inventor 2015
Message 8 of 13
Curtis_Waguespack
in reply to: crev64

Hi crev64,

The file called part.ipt is not a solid file, it is a composite surface. To convert it to a solid, use the Stitch tool and select the composite (or any face of it), this should turn it into a solid. Once that is done you can use one of the workflows mentioned before to cut it from the other part.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 9 of 13
johnsonshiue
in reply to: crev64

Hi! Here are two workflows that you might consider

Derive Assembly:

1. Start a new part.

2. Derive -> pick the assembly -> Derive Style = Single Solid Body; PART:1 = '-'; BLOCK 1_S:1 = '+' -> OK.

The result should be a new part containing a block body with PART:1 body cut away.

 

Copy Object:

1. Open the assembly containing the two parts.

2. Edit BLOCK 1_S:1 in place.

3. Copy Object -> associative -> pick PART:1 -> OK.

4. Stitch the copied body.

5. Combine -> pick the block body as base and the stitched body as tool -> Cut ->OK.

The result should be the block body having PART:1 body cut away.

 

Please let me know if you have any question using above workflows.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 10 of 13
crev64
in reply to: Curtis_Waguespack

I can't seem to get it to stitch together. What I sent was a small portion of the overall part (and a fairly simple part too). When I try to do it to the whole thing, the program always freezes and crashes. I can make it more solid by opening the part, clicking copy object, and making it into a composite or a series of surfaces. That's all I can really do with it.

Crev64
Autodesk Inventor 2015
Message 11 of 13
Curtis_Waguespack
in reply to: crev64

Hi crev64,

Can you zip and attach all of the portions? If so I'll try and have a look and if I can get it converted to a solid, I'll post it back as a STEP file since I don't have Inventor 2009 installed any longer.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 12 of 13
jletcher
in reply to: crev64

Here is your part in step format just import it and do the derivd component.

 

I did it to make sure it worked and it did..

Message 13 of 13
karthur1
in reply to: crev64

 

When you use the sculpt tool, I take it you have selected to "remove" material. Try changing the direction to see if it makes a difference. On something simple its pretty intuitive, but if you have multiple surfaces, it gets tricky as to which way it should go (at least for me anyway).

 

There will be a little green arrow on the surface showing you the direction.

 

2013-03-21_1119.png

 

 

Kirk A.

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