relax found relationship issues

[multicaduser]

Using the new sketcher in NX 2212 I'm having issues relaxing found relationships. More specifically, two lines that have a found colinear relationship. First select the line and the relationship appears, second select the relationship to relax, third drag the line. Problem is the relationship turns magenta supposedly indicating the relationship is relaxed, but when the line is moved the other follows.

The above example exactly follows a help video that comes up when help is activated in the sketch command. Are there options that must be set, is this a graphics bug or maybe just a bug? Any ideas, suggestions or videos would be welcome because this is killing my productivity.

tia



NX 2212 Windows 10

 

[AZPete]

The new convention is that dimensions override implied (found) constraints. Not exactly certain of HOW to do it, but there is a "shake" method that seems to drop the found constraint and allows the object to be manipulated as an isolated item. The HOW is uncertain because trying it is infrequent and getting the knack isn't natural. But, grab the item and shake it. See if that works. Otherwise, override by applying dimensions so that the constraint loses priority.

 

[multicaduser]

Thanks AZPete, but shaking will remove all the constraints and only the colinear needs to go. Right now I either shake or delete and start over. Mostly wondering if there is some setting that is missing to not make it work like the video in the help.

NX 2212 Windows 10

 

[AZPete]

Part of the problem with implied constraints is that you don't get asked if you want them. So, when you have an incidentally coincident line, you need to lock one in place so you can move the other without it tagging along uninvited.

The lesson learned from experience in this is that one needs to be explicit in constraints so that the behind the scenes interpreter doesn't assign undesirable constraints. Start out the sketch making orthogonal features truly orthogonal and locked to or parallel to their axes. Have been told that is unnecessary, but also have found that down the road when edits are made and the model behaves "unusually", it likely stems from not being nailed down "correctly". So, start by nailing everything down the way you want it. Moral of story: new method requires vigilance and therefore near 100% specificity--seemingly obviating the short cut "ease" of the new sketch paradigm.

 

[multicaduser]

AZPete, thanks for the reply, I agree with what you say and have actually been doing that. I found out the issue with this particular sketch was that an inferred mirror relationship was added to another set of lines attached to the first set using dimensions. This mirrored relationship had nothing to do with the first set of lines directly but affected them just the same, so relaxing the inferred colinear relationship didn't work until the inferred mirror relationship was removed.

I would like to see an option to show all the inferred relations without having to pick the entity so they could be selected and relaxed, especially if there are multiple relations that need to be relaxed. Not knowing what relations the sketcher thinks you want is a bad way to work, it's like feeling your way through a room blindfolded.

Another option would be to just turn off inferred altogether. Depending on the design process they can be beneficial or a huge hinderance. I find that that inferred relations break too easy, and for the wrong reasons, imho, so I tend to add persistent relations where possible.

NX 2212 Windows 10

 

[AZPete]

Shortcuts are great until you end up in the wrong place. Taking the correct route doesn't allow a shaving of time, but you GET there and on time.

Be aware that the mirror sketch function has an option to turn on the hard relations. If that is not toggled, one can create a symmetry of sketch only to watch it fail to maintain symmetry upon dimension editing. Very confusing until one understands the toggle available. After all, one would probably universally assume that to command a symmetry within geometry means: "stay symmetrical!", but that's not the case. The option allows more freedom to decide and manipulate, for certain, as it can be ON or OFF instead of always ON, but it can catch the unwary/untrained by surprise.