UNION tool bugs?

Jim Canale

I was just wondering if anyone but me is having intermittent problems with the UNION tool.   Unless the parts I am joining are very simple in shape, I sometimes wind up with lines where the parts join.  The CLEAN tool doesn't remove the lines.   The lines appear on the 2D drawing views too.   Some times, parts union together very cleanly.  Other times, the lines appear.   Anyone have any idea what causes this, and what to do about it? 

Jim Canale

Here are some screenshots of the issue....

Union not exhibiting the problem.jpg

Unwanted L Shaped Line.jpg

Line on Generated Views.jpg

Roy Klein Gebbinck

You should check if the surfaces are exactly coplanar.

Jim Canale

@Roy Klein Gebbinck:

You should check if the surfaces are exactly coplanar.

I have.   I have also submitted a support request.  They responded that I should change my visual style.  But all that did was hide the line from view.  It appeared again on the 2D generated views.  It is confusing to the job shops that will build the part.

Jason Bourhill

Hi Jim,

I think Roy's comment is likely to be correct, however you may not be able to see it with the units settings of your drawing. Starting with the two components you want to union, I would try the following:

1. Set LUPREC to max value of 8.
2. Scale the two parts you want to union up by a large factor, such as 50,000.
3. Using inquiry tools (_DIST, _ID) compare the parts around the union point.
   

If you see differences between points that should be identical, or should have the same X, Y, or Z, then the surfaces aren't coplanar.

Regards, Jason Bourhill CAD Concepts

Roy Klein Gebbinck

@ Jim: Can you post a drawing?

Jim Canale

@Jason Bourhill:

Hi Jim,

I think Roy's comment is likely to be correct, however you may not be able to see it with the units settings of your drawing. Starting with the two components you want to union, I would try the following:

1. Set LUPREC to max value of 8.
2. Scale the two parts you want to union up by a large factor, such as 50,000.
3. Using inquiry tools (_DIST, _ID) compare the parts around the union point.
   

If you see differences between points that should be identical, or should have the same X, Y, or Z, then the surfaces aren't coplanar.

Regards, Jason Bourhill CAD Concepts

Jason,

Thanks for your reply.  I set LUPREC to "8" and scaled the parts by a factor of 50.   I only checked a couple points along the top of the parts, but didn't detect any differences .    I created the part outlines on the same plane, and extruded them to the same exact thickness.  So I'm not sure how they would become "non-co-planar".     I'm also not sure what I would do to correct it if they were.   Would 3D rotate be of sufficient accuracy to bring the parts co-planar for a proper union? 

Jim Canale

Sorry I forgot to post it Roy.  Here is the drawing showing the parts before the UNION operation.. 

I highlighted the short part in red.    In the lower view, I overlapped the parts.   I thought the overlap might be causing the problem so I shortened the long part and butted it up against the short part.  Neither unioned properly.

Union not working.dwg

Roy Klein Gebbinck

Jim, as suspected the top planes of the solids are not coplanar.
I have switched the LUPREC to 8 and have used the _ID command to check the corners of the top planes of the assembly without overlap.

The points of the white solid are (Starting at the lowest X and Y, and going CCW):
[code]: ID
Select point to identify coordinates:
 X=-54.74839018  Y=117.55505048  Z=0.00000000
: ID
Select point to identify coordinates:
 X=204.00160982  Y=117.55505048  Z=0.00000000
: ID
Select point to identify coordinates:
 X=204.00160982  Y=191.55505048  Z=0.00000000
: ID
Select point to identify coordinates:
 X=-54.74839018  Y=191.55505048  Z=0.00000000[/code]

The points of the red solid are:
[code]: ID
Select point to identify coordinates:
 X=-85.99839018  Y=88.43005048  Z=0.00000005
: ID
Select point to identify coordinates:
 X=-54.74839018  Y=88.43005048  Z=0.00000007
: ID
Select point to identify coordinates:
 X=-54.74839018  Y=191.55505048  Z=0.00000000
: ID
Select point to identify coordinates:
 X=-85.99839018  Y=191.55505048  Z=-0.00000002[/code]

Louis_Verdonck

 Dear Jim

the problem in the model is that the top face of the red solid is not perfectly level. There is a difference of 0.00000007 drawing units between front and back (smallest faces). To test this yourself, set LUPREC = 8 and draw a line along the long edge of the top face. Then select the line and check the Delta Z value in the Properties Bar.

Jim Canale

Louis,

So how do I correct it?

Joe Dunfee

 One possible solution is to create a box large enough to cover the entire solid model. then move it so that you can subtract it from the original part, and thus get rid of the problem surface.  You have to move so that you end up with a known thickness.  

E.g. you want the finished part to be 1/2" thick. Then, you do your subtraction so that the part is 1/4" thick.  After that, you must offset, or extrude the finished surface 1/4" to end up with your part at 1/2" thick.

-Joe

Joe Dunfee

 I just looked again at the original part, and you don't have much space to work with, but since the problem is fairly shallow, you only need to subtract a small amount of material. You might subtract only .01" of material.  If you move the resulting face out by 0.01" then even the chamfer will maintain itself.  

Note that extruding the face is NOT the correct action to take, since the chamfer will not be preserved.

-Joe

Richard Webb

Here's my stab at it.

You can use a coincident constraint (dmCoincident3d) to get faces on the two objects aligned. However, you want the complete objects to move, not just faces. So first select each of the two objects, individually, and apply dmRigidSet3d to each. That locks them so that all elements of each object move together.

Now we could apply coincident here but it seems that the two are so nearly aligned that coincident misses it. There's probably a variable somewhere which could be set to allow this step to be skipped, but this works: rotate the smaller object some nominal angle around the X axis to make the misalignment between the two "big enough." I used 30-deg. Now apply a dmFix3d constraint to the larger box to hold it in place and then a coincident constraint between the top faces on the two. That makes them flat together. Do the same to the two rear faces to line them up as well and that completes the alignment.

Jason Bourhill

Hi Joe,

I think Richard is on the right track in using 3D constraints. Prior to applying UNION you could use 3D constraints on your parts to ensure that faces are perpendicular, parallel etc. These constraints should correct any discrepancies with the parts. Then using constraints again to align correctly for the union operation.

Regards, Jason Bourhill CAD Concepts 

Jim Canale

Thanks, Louis, Joe, and Richard,

All good ideas, but I'm going to use Richard's approach.  I have been avoiding learning how to use the constraints, since I played with them in V13 and they seemed buggy.  But I just did another project that required me to place one flange of a piano hinge on an angled surface.  Worked great!    The way I was trying to do it was tedious and error prone.

Anyway, I'd still like to know how the part became non-coplanar.   

Jim Canale

Ooops!  Didn't mean to forget to thank you Jason!   Great support from everyone as usual.  I'm old and a slow learner, but I hope someday I can help someone else out here, and pay back the favors.

Patrik Sparrman

My method was to make a new box place it on the 0.0.0 corner move it down 0.1 and then subtract it. Finally Push/Pull the Surface up 0.1 to preserve the chamfer.

Worked nicely.

Jim Canale

@Patrik Sparrman:

My method was to make a new box place it on the 0.0.0 corner move it down 0.1 and then subtract it. Finally Push/Pull the Surface up 0.1 to preserve the chamfer.

Belated thanks Patrik.  I am going to bookmark this thread, as it is all very good information.