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NX 10 Constraint problem behavior

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06-08-2017 07:35 AM

Can someone please help? I am trying to assemble a component/part next to another part. I am using the coordinate systems of both parts and a vertical surface of each part to assemble to each other. I'm using Align of the XY and ZX planes and then using Touch of the vertical surfaces of the parts to get the surfaces to actually touch together. I've been able to do this countless times and then it fails with this one. Is there some variable or setting that I'm missing? I've spent more than 10 minutes trying to do a "simple" task that should have been a non-issue.

I can align both planes and everything is OK, but then it fails when I try to touch the two surfaces together. I can also touch the two surfaces together, but then it fails when I try to align the planes. I checked the angle of the coordinate system planes to the vertical surfaces and they show as 90 degrees. Everything seems to line up exactly, but it doesn't work.

After fighting this for 20 minutes or more, I eventually added a distance constraint from the YZ plane of one part to the vertical surface of the other part. That "worked", but I have no idea why this was such a problem. Any help would be appreciated. Thanks

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Re: NX 10 Constraint problem behavior

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06-08-2017 08:27 AM

One possible reason is due to the NX tolerances and degrees of freedom. If you constrain a plane to plane you have these two surfaces parrallel and touching. Now you try to make two centerlines coincident and parrallel and due to NX tolerances these are not exactaly 90 degrees to the planes constrained. We have had this issue back in the old I-Deas days. We find this happen to us every once and while and we could not figure out why most of the time doing what you did work. Then sometimes we have to use the point on axis to fix it.

Try using a point from the coordinate sysem and touch the coordinate system axis. This may work. good luck

Re: NX 10 Constraint problem behavior

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06-08-2017 08:39 AM

It seems redundant to align the planes AND touch the surfaces. Why not just use touch on the surfaces and leave it at that?

As for your problem, I'd guess that one (or both) of the planes is a small distance away from the surface which is preventing both constraints to be satisfied simultaneously.

Re: NX 10 Constraint problem behavior

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06-08-2017 09:04 AM

I'm using the surfaces and the planes because the two parts that I'm assembling next to each other are actually not the same part. I just showed a screenshot of one of the parts to show the coordinate system planes and surfaces that I was mentioning.

For this comment: "As for your problem, I'd guess that one (or both) of the planes is a small distance away from the surface which is preventing both constraints to be satisfied simultaneously."

- I have the coordinate system in the middle of the part, so they aren't touching the vertical surface of the part. Does the plan have to go through the vertical surface? I think I've assembled parts that were big and the coordinate system plane did not go through a vertical side. Maybe I'm not understanding the comment correctly.

For this comment: "One possible reason is due to the NX tolerances and degrees of freedom."

- Do you know if these limitations are being addressed in NX 11 or later versions? NX is a lot more of a "fragile" software than what I'm used to working with, so hopefully this can be fixed/improved. Thanks

Re: NX 10 Constraint problem behavior

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06-08-2017 09:17 AM - edited 06-08-2017 09:22 AM

Re: NX 10 Constraint problem behavior

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06-08-2017 09:22 AM

Re: NX 10 Constraint problem behavior

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06-08-2017 09:25 AM

Re: NX 10 Constraint problem behavior

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06-08-2017 09:40 AM

@s_hightower wrote:

- Do you know if these limitations are being addressed in NX 11 or later versions? NX is a lot more of a "fragile" software than what I'm used to working with, so hopefully this can be fixed/improved. Thanks

Having been working with new to NX users, as the company moves to NX, I have heard similar statements a lot. After looking at both sides, I don't see that NX is more fragile, but less "forgiving", due to the accuracy. I think other software has included more tolerance, or "fuzziness", which allows the user to just be close. NX is not like that. There is a .001in modeling tolerance, and if things are out of tolerance due to rounding, tolerance build up, etc., it still holds you to it.

Uisng points, and the Angle constraint with the orient option, will help.

-Dave

NX 11 | Teamcenter 11 | Windows 10

NX 11 | Teamcenter 11 | Windows 10

Re: NX 10 Constraint problem behavior

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06-08-2017 09:45 AM

Based on your post and picture, here is the situation as I understand it:

You have two parts, each with a datum csys near a planar face. When positioning these components in an assembly, you are using align to align the planes of the coordinate systems (either to each other or to a csys in the assembly) and then using touch on the planar faces. If this is the case, I don't understand why an "align" AND a "touch" constraint is necessary. It seems that "touch" would suffice. Additionally, if the plane of the csys is a small distance away from the planar face (greater than the constraint tolerance distance), you would be able to apply either the align or touch constraint, but not both. Align and touch both create a coplanar condition; all the objects (2 planes and 2 surfaces) would have to satisfy that constraint. If the csys and surface are in the same file, they move as one unit; if these are not coplanar to start with, you will not be able to satisfy both the align and touch constraint.

Please clarify if I have misunderstood.

Re: NX 10 Constraint problem behavior

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06-08-2017 10:19 AM

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