Can't dimension Sketch to datum plane

[Buckshott00]

Hello,

I am running NX7.5.4.4 on Windows XP Pro 32bit.

One of my settings is off. When Sketching I am unable to dimension to a plane. When I save a part on our network if another engineer opens the the sketch they are able to dimension to the plane, but I am unable to.

I have looked at the selection filters but I turned them off and still have the problem

 

[jerry1423]

Check your filer setting. I try to have mine always set to "No Selection Filter" . . . yours is probably set to either "curve" or "sketch"

 

[Buckshott00]

negative, I said it at the bottom of the post. No selection filter is on, and the selection scope is withing the active work part.

 

[JohnRBaker]

This is a single piece part (not an assembly), correct?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[Buckshott00]

Correct,

It is a single piece; however, it's body is waved linked back to another part. Aafter the linked body the references are shut off.

I have found that if I delete some center-lines in the sketch the issue is alleviated.

However, the center-lines were created in the sketch and fixed there was only 1 dimension to 1 of the center-lines but it would not let me select any plane to dimension to.

 

[JohnRBaker]

Check your Load Options to see if there is a difference in the settings, particularly with respect to 'Partial Loading' and 'Load Interpart Data', between yours and the other systems where the problems are not occuring.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[Buckshott00]

Okay I checked it against a coworker's pc and his assembly load options are the same. Is there another set of load options I am supposed to check.
What I checked: File > Options > Assembly Load Options

 

[Xwheelguy]

I noticed that I had to have my dimension set to either Inferred or Perpendicular before I was able to select a Plane. Horizontal or Vertical doesn't work.

Tim Flater
NX Designer

 

[Buckshott00]

Xwheelguy,

I tried that too. I have tried parallel perpendicular inferred horizontal and vertical when I deleted out 1 of the center-lines I was able to use the inferred dimension, but it gave me an angular dimension to the line I selected, I tried selecting the end point of the line, but it would not allow me to place a dimension with that

 

[Xwheelguy]

I would try making a new part, then immdiately creating a sketch with Datum Csys then throw in some curves and save the file to the same network location....see if you can dimension to the datums then.

If not, then it might be isolated to the part file or something in that particular file is the culprit.

That would tell you about a setting/default, at least on new parts.

Tim Flater
NX Designer

 

[Buckshott00]

Yeah, that where things get interesting. I have already moved past that part, but I am trying to solve why it is doing that because it has been a problem for me and no one else in the office.

I tried putting in a CSYS at absolute, and moving it to the top of the part history, even before the linked body. Then I set the sketch to the current feature. At this point I am still unable to dimension to any planes with any type of dimension. Then if I reattach the sketch to a plane on the CSYS I am unable to dimension from any of the planes, but able to dimension to the CSYS. All of the datum planes and fixed datum planes higher on the part history are unable to be selected.

It is some setting file but it has to do with how I am making sketches that is different than how everyone else is.

 

[mmauldin]

Just to let you know, you are not the only one to encounter this. I've had it happen a few times, very randomly. I wish I could tell you what the problem was but I have never been able to figure it out. I just deleted the offending sketch and recreated.

 

[wackolacko]

Are you doing 'Direct Sketch' or 'Sketch in Task Enviroment'?

John Lackowski
Onsite Level 2 NX Support
Chrysler
800 Chrysler Drive, Auburn Hills, MI

 

[Buckshott00]

Wackolacko,

I have tried it both ways. This latest one I believe is Sketch in Task Environment

 

[JohnRBaker]

I think it's time you contacted GTAC and have them look at this, although if it appears to be specific to one workstation as opposed to another, they may not be able to help if they can't actually reproduce the behavior that you're seeing, but it's worth a shot.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[Buckshott00]

Thanks John,

I will send the part to GTAC and explain.

 

[jerry1423]

Make sure the layer that the datum plane is in is "selectable".

 

[Buckshott00]

jerry,

yes the planes are selectable, this problem only happens when I am in the sketch

 

[Buckshott00]

Just got the solution from GTAC. A positioning dimension was in use. If a positioning dimension is in use then you cannot place sketch dimensions.

Thanks for everyone's help on this.

 

[JohnRBaker]

Ah yes, I forgot about those. This is a leftover concept from when sketches were treated as as a single 'rigid body' relative to the other objects within the part file and therefore you needed special 'Positioning Dimensions' to define where a sketch was located relative to other objects in the part file. Several releases ago we enhanced 'Constraint Dimensions' so that you could use them to reference objects outside the Sketch as well those inside the Sketch. Of course, if you're going to allow users to individually constrain Sketch curves relative to non-sketch curves, this would be in conflict with the idea that I was positioning the entire Sketch as a single object, which is what you're in essence doing when you use explicit Positioning Dimensions. Granted, we could have removed the idea of using Positioning Dimensions altogether, but at least at the time, there was a thought that since this had been a standard feature for locating a Sketch, that we would leave them in but promote the idea that you don't need to work that way since using only Constraint Dimensions provided more capabilities and flexibility, however that did mean that users would have to be prevented from attempting to apply BOTH Positioning Dimensions as well as Constraint Dimensions, between Sketch curves and non-sketch curve/objects. It's this 'lockout' that tripped you up.

As for what to do in the future, in all honesty, I think you will be better served simply avoiding the use of Positioning Dimensions and depend only on Constraint Dimensions. In fact, out-of-the-box the Positioning Dimension icon is hidden and must be explicitly enabled before you can even apply any and with the new 'Direct Sketch' functionality, Positioning Demensions are not even an option as they've been removed altogether when working in that mode.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.