NX12 Substract body 2

[NX10user]

Dear Users,

I want to do a subtract boolean on my model in NX12. I have two solid intersecting bodies, but I cannot perform it as it gives an error which prompts me to "examine geometry". How can I get over this error? I have uploaded my part file. The part is generated externally and then uploaded in IGES format into NX12.

Thanks in advance.

Please find the link to the file:

http://files.engineering.com/getfil...d-41cd-a2bc-443cfd905227&file=Single_Yarn.prt

 

[jerry1423]

Can you post a parasolid of this file ?

Jerry J.
UGV5-NX11

 

[cowski]

If it prompts you to "examine geometry", one or more of the bodies probably has geometry errors. After importing the IGES, try using "heal geometry" and/or "optimize face" to clean up the geometry. If this can't clear the error, you may need to make some changes to the process that generates the geometry.

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[Rob_N]

In this case, both of your "solids" are too close to the same size.
they share common outer walls the would end up making a zero thickness problem. NX doesn't like that.

If you make the box smaller or bigger, you can subtract the airfoil shape from it.

 

[Toost]

A few notes.
This model is very small, 1.72 mm the longest side. I hope this is as expected and not a translation error.
It consists of two main features, a freeform shape and a block.
The freeform should be subtracted from the block.
Since the bodies were imported, we know nothing about the accuracy of the respective body. . - the "block" consists of 6 sheets which have been sewn together.
The freeform shape is more complex than necessary for the shape, its single face is 3x3 degrees and 30x36 patches. ( what system is the origin of this ?)

In this case, the message in NX 12 is that the flat faces in the end of the freeform is intersecting with the flat faces of the block. This condition is very difficult for a solid modeler to calculate.( no matter what system we speak about, it is not a NX specific issue.) imagine two objects without thickness , in 3D space, which lie in almost the same plane, then one face ( still without thickness) should be subtracted from the next. Had the ends of the freeform extended outside the block with any distance, the operation would have been done in no time.
In this case, there is a neighbor face which is touching the face of block, but still fully enclosed.
See image below.
In this case, if you increase the tolerance of the intersect feature to 0.02, it will finish.
( NX will allow that enclosed face to cut the block open using the tolerance.)
Another method could be as like in the uploaded example. Using the Patch feature.
The patching tolerance will allow the " wobble" and the deviation that the freeform faces edges has to trim to the planar faces of the block.
see the section curves in the attached part, there is a tolerant gap.
This is still a watertight solid. Fully valid.


Regards,
Tomas

 

[NX10user]

Dear All,

Thank you for the kind suggestions.

Tomas, the model is indeed small and is not a translation error. The model originated from a composite modeling software called as TexGen. The dimensions of the part file are as specified and required. The freeform shape is more like a yarn embedded in a matrix( here block) of a composite. After investigating the geometry, it seems that 2 parts viz: freeform and block are exported as sheet body. I think subtract boolean operation cannot be used on sheet bodies? Its like subtracting 0 form 0.

I tried to convert the bodies into solid by "Surface -> Sew operation" and then used the subtract boolean operation, the error of examine geometry pops ups. But now, the patch option also looks a sustainable option. I'll try this option on the actual geometry (much more complex model) which needs to be modeled and then let you know if this works or not.

 

[cowski]

I think subtract boolean operation cannot be used on sheet bodies?

This is correct. A sheet body cannot be the target or tool of a subtract operation.

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[Xwheelguy]

However a sheet body CAN be used in a similar manner as Subtract using the Trim Body command....same general rules will apply regarding the tool passing through the target such that a volume is being removed.

Tim Flater
NX Designer
NX 11.0.1.11 MP4
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[Toost]

hm , fellows, fellows...
A sheet body can be the target body for a subtract operation and Intersect. ( You can subtract a solid body from a sheet)
A sheet body cannot be used in the Unite feature.
A sheet body cannot be the tool in any boolean. ( One used to be able to subtract sheets from solids, ( same result as split )but that isn't possible anymore.)

Regards,
Tomas

 

[cowski]

Thanks for the correction, Toost. I've edited my previous post.

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[NX10user]

Toost aka Tomas, you are just too good with NX. Kudos.

Just an additional question. Is there also a way to make a negative CAD in NX.

I have tried to make the freeform shape as a solid body by sewing the sheet body shape but I would also like to fill the bounding box and behave like a solid body. The only condition that it should account for another solid body here freeform shape while filling. What are your thoughts?

 

[jerry1423]

You can thicken the freeform shape.

If the rectangular cube is actually a solid body you will want to a Replace Face
You will replace the top face of the rectangular cube with the freeform shape.
If you do this it is always a good idea to make the freeform surface bigger than the face of the rectangular box.

Jerry J.
UGV5-NX11

 

[cowski]

You can also use the "trim body" command to trim a solid body (such as a block) with a sheet body (such as the "freeform shape" in your screenshot). To be successful, the sheet body needs to be larger than the solid. In the screenshot above, the trim body command would probably fail as it appears that the block is wider than the freeform shape.

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