Error: The Tool & Target Do Not Form A Complete Intersection

[BrittToolEngineer]

I have a solid body where I've been putting .250 dia holes thru the body of a tab. Some of the holes went through and inserted just fine. Now I have a hole that gives me the error in the subject line. Can anyone help with this problem?

Thanks in advance,

Brent

 

[NutAce]

How are you creating these holes?
And can you post the part?

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[BrittToolEngineer]

Hi Ronald,

I'm using the Hole command and putting in a general hole using a projected curve centerline as the axis for the hole. I am new to the software, 2 months in right now, so I'm not sure what posting a part means. I can tell you that I created my file from a parasolid from our customer. It is a thin part that is laser trimmed. Our fixture holds this part that has tabs around the perimeter. When I started putting holes in the tabs, the very first hole, the hole was too close to the outside boundry, but the hole still went in successfully. I just simply moved face to give the tab more geometry for the hole. But when I went around the corner to another tab, I started getting this error. I moved the face eventually, and the hole went in just fine. I wonder why the first hole went in and some did not with not having the geometry.

Anyway, I think I have the problem solved. Just trying to learn what happened to create the error.

Thanks,

Brent

 

[NutAce]

Without having a look at your model it is difficult to find the cause..That is why I asked you to upload your model (part) to this thread...Then we can have a look at it.
Most probably it is the projection which is causing a problem. What is the reason you are using a projected curve and not just a normal vector for the hole?

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[BrittToolEngineer]

I'm being coached to do the projected curve. I believe we did this due to using the customer's part to project holes where we will install in our fixture in order for the end user to laser cut their holes. So it is simply a projection from a part that is our guide in building the fixture.

I apologize in advance; however, it is not legal for us to send these part files to anyone but the customer.

 

[BrittToolEngineer]

Pardon me Ronald, we used a virtual curve, not projected, and basically it gave us a centerline for all holes at the location and angle of that hole. There are many holes and each one is a compound angle and all different.

 

[MFDO]

Brent,
Check the following in the Hole creation Window:
Hole>Form and Dimensions> Depth Limit> THRU BODY
Hole>Settings>Extend Start> YES

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[cowski]

When boolean operations don't work as expected, the first thing I do is run the "examine geometry" command. Turn on all the body and face checks then window select around the entire model and press the examine geometry button. If any of the body checks fail or if the face self-intersection test fails, later operations may fail (such as booleans). The window select (or rectangle select) is important because it will pick up the body itself, all the faces, and all the edges. If you single pick on the body, then only the body is selected and analyzed; no tests are run on the faces or edges in this case.

When working on imported geometry (you mention a parasolid file from your customer), the first thing you should do after import is run the examine geometry command to ensure that you are starting with good geometry. I would also recommend running the "optimize face" and/or the "heal geometry" commands before starting work on the imported geometry. These commands can help clean up minor geometry problems in the file. If, after running these commands, examine geometry still shows errors (body consistency being a big one); I'd suggest contacting the customer to see if they can clean up the file and try again or try a different export format.

www.nxjournaling.com

 

[BrittToolEngineer]

Very good information and advice. I thank you so much for your assistance.

 

[MFDO]

Cowski, Now I try to stay away from those optimising commands. I find it creates more problems in downstream operations especially in CNC programming crating unmachinable /unrecognizable surfaces. Now what I do is Examine Geometry, Delete Face and Fill Surfaces (patching up).

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[cowski]

Have you tried them? What optimize face does, is convert B-surfaces into analytical geometry if they are within a certain tolerance. If anything it would make it easier to use in downstream operations.

www.nxjournaling.com

 

[MFDO]

Surely I tried them, sometimes over and over again while fixing faces. Maybe I over used it to screw up the desired/allowed watertight surfaces, CNC tolerances and gaps. Anyhow it created problems and since I avoided them, didn’t hear any complains.

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks