Unite solid body
Unite solid body
(OP)
Hi
I have problem with unite two bodies which are close together. When I use tool unite I get error :
"Thru face does not intersect path of the tool".
Could you please, some one help me to do combine these bodies. Thanks advance.
Velto
I have problem with unite two bodies which are close together. When I use tool unite I get error :
"Thru face does not intersect path of the tool".
Could you please, some one help me to do combine these bodies. Thanks advance.
Velto





RE: Unite solid body
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
http://www.siemens.com/ugs
http://www.plmworld.org/museum/
RE: Unite solid body
Velto
RE: Unite solid body
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
http://www.siemens.com/ugs
http://www.plmworld.org/museum/
RE: Unite solid body
You could try selecting the tool and target solid in the opposite order, in some cases that helps.
When models are booleaned meaning united subtracted or intersected, then think of it as trimming and sewing the elements together. You could have two faces that appear to be touching without having the two solids overlapping into one another, so that you have to ask yourself whether you could trim and sew those faces within the modeling tolerance to get a valid result. Several things can affect this depending on how your geometry was created. It is too hard to predict very much without seeing your model.
If as a part of the unite one of the solids will join the other in more than one place then you might try to analyze the problem. You can do this by trimming away half of both bodies to a plane then attempting to unite the remaining sections. If it works you know then problem is likely to be on the opposite side of the model. Afterward reverse the trimming side to retain the other half and try again to prove your analysis. Sometimes you will repeat this several times to zoom in and discover the site of the problem.
From time to time you can simply offset a face to create a sure fire intersection of two solids and improve your chances of having a unite work properly.
If all else fails post your model to www.yousendit.com and publish the link here so one of can diagnose and maybe fix it for you.
Hope this helps
Regards
Hudson
RE: Unite solid body
One more thing. Please Perform an analysis>Examine geometry check of your model. If you have self intersection or consistency errors in your model then that will affect often affect your ability to boolean.
As part of that check is output to the information window then if you're not sure about what you have then you could capture the results and post them in a reply.
Regards
hudson
RE: Unite solid body
http://download.yousendit.com/0A76F93D7DD72F7E
Could you please see it and give me some advices. Thanks again
Velto
RE: Unite solid body
Anyhow, I was able to unite the two by offseting the datum plane slightly in each direction, trimming the solids back to their relative planes and then adding a positive offset face to each. They then both had planar surfaces (which were absent originally) and united correctly. Due to the way this part is constructed, the offset size doesnt matter as long as it is large enough to meet the datum plane betweeen the pieces. The offset wouldn't go beyond the datum plane between them.
I am sure that there are other ways to accomplish this, but I am still somewhat unfamiliar with NX5 and need to get back to work...
RE: Unite solid body
Velto
RE: Unite solid body
The parent data will control the boundary of your faces, so no info is lost.
RE: Unite solid body
Velto