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Unite solid body
- Thread starter velto
- Start date
JohnRBaker
Mechanical
You have a slight misalignment where the two bodies are not quite touching. Try moving one of the bodies toward the other a very small amount and reattempt the Boolean ADD.
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
- Thread starter
- #3
Thank you very much for your fast reply JohnRBaker. I have tried to do according by your instruction but it is still same problem. I want to show you screen shots of my computer but. I don't know how I could post the picture in this forums?
Velto
Velto
JohnRBaker
Mechanical
OK, try editing (make larger) at least one of the solids so that it intersects the other.
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA
Velto,
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 and publish the link here so one of can diagnose and maybe fix it for you.
Hope this helps
Regards
Hudson
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 and publish the link here so one of can diagnose and maybe fix it for you.
Hope this helps
Regards
Hudson
Velto,
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
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
- Thread starter
- #7
Thank you very much for for your help John and Hudson. Here you can see my project on:
Could you please see it and give me some advices. Thanks again
Velto
Could you please see it and give me some advices. Thanks again
Velto
You should have mentioned that this is in NX5.
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...![[peace]](/data/assets/smilies/peace.gif "[peace] [peace]")
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...
- Thread starter
- #9
Sorry Ewh I still understand you how I can trim the body by datum plan without losing parent data.By the way I created these bodies by sewing surfaces around. I had tried to extrude surface of the small body slightly to the big one then unite with the original, after that I unite two bodies but it was still same problem. Could you please tell me more detail your trick. Thank you
Velto
Velto
When you sewed the body together, you did not get planar faces or definite edges, but some sort of small radii (which will prevent offsetting the face you need). Therefore, you need to trim the body back to a plane giving you definite planar edges and surface. Offset the face to its original location and the resulting face will also be planar. Do this to both bodies and they will unite.
The parent data will control the boundary of your faces, so no info is lost.
The parent data will control the boundary of your faces, so no info is lost.
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- #11
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