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strange behavior of sketch

Valued Contributor
Valued Contributor

Hi together,

 

have someone experiences or can explain of this situation?:

Two sketches, both are copy of one. But one has standard normal orientation(Y is vertical up, X horizontal right,Z is straight out of screen) and second has practical XY directions inverted (Y is vertical down, X horizontal left,Z is straight out of screen). After all this, by function "orient view to sketch" both have orientation of view same (see Attachments).

Is possible to turn wrong sketch back to standard?

 

Thank you for reply.

9 REPLIES

Re: strange behavior of sketch

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

You could try Reattaching the inverted sketch.  Right click the inverted sketch in the Part Navigator and select "Edit Parameters".  Select the Reattach icon and note the Reverse Direction and Reverse Side options.  You can also redefine your Horizontal/Vertical Reference.  This might give you the control that you're looking for.

 

Regards, Ben

Re: strange behavior of sketch

Valued Contributor
Valued Contributor

thanks, but I tried it.

The core of problem is on both pictures to see.

Standart behavior of function "Orient View to Sketch" is, that orients in view where x goes to right and y goes up. But by this broken sketch is all inverted. Why?

Re: strange behavior of sketch

Phenom
Phenom
Would it be possible to upload the part with sketches?
Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: strange behavior of sketch

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

Orient view to Sketch will orient the view to whatever is defined as the horizontal or vertical direction in the Sketch.  If you select "Edit Parameters > Reattach" you will see a vector indicator in your graphics display showing you the current reference.  Take a look at the attached movie, you'll see that my horizontal direction is defined in the opposite direction to my X-axis.  When the sketch is originally activated the orientation is the same as your inverted image.  Once the direction is reversed the X-axis and Y-axis display as you're expecting them to be.

Re: strange behavior of sketch

Valued Contributor
Valued Contributor

 

Gotcha!?!

 

By Sketch are two independent directions. One is of View Orientation and other is for sketch.

thought, there is only one.

Unfortunatly, this is not solution. It move problem to lower level of sketch definition.

 

In Attachment are pictures to compare between both sketch definitions and also Part with sketches.

 

Best Regards

Re: strange behavior of sketch

Phenom
Phenom

RMB the Sketch, one at a time and select “Make Datum External”

Double click the wrong orientation datum and redefine it to correct orientation.

RMB the Sketch, one at a time and select “Make Datum Internal” (To hide WCS)

Fix the wrong sketch Dimension line.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: strange behavior of sketch

Valued Contributor
Valued Contributor

Thanks both gentlemans for solution.

First time the solution from Mr. Fernando didnt function.

So i make a synthesis.

 

Also i did it so:

1) BenBroad:

 

RMB on sketch and "edit parameters" and revers direction

 

then

 

2) mike_fdo:

RMB the Sketch, one at a time and select “Make Datum External”

Double click the wrong orientation datum and redefine it to correct orientation.

RMB the Sketch, one at a time and select “Make Datum Internal” (To hide WCS)

Fix the wrong sketch Dimension line.

 

It works.

 

Now question: how can man avoid this situation? For some months inverted sketch wasnt inverted, but only standard orientation and only supressed by expresion. 

Re: strange behavior of sketch

Phenom
Phenom

 

Now question: how can man avoid this situation? For some months inverted sketch wasnt inverted, but only standard orientation and only supressed by expresion. 


Pay some special attention to Create Sketch window’s “Plane Orientation” and Select Reference X or Y accordingly to Reference Selection.

In the first sketch, make the first sketch datum external. It will give you an idea about the orientation.

Note: Avoid or hide that DCS to refrain from using this DCS as next sketches’ plane reference; otherwise you will not be able to make it (first; the new parent) internal datum again. While in the Create Sketch window you could RMB the DCS to show/Hide as needed.

Optionally you could have one DCS(External) serving as a common WCS. RMB the second DCS and select “Replace” with the first.

There are many of other options too.  

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: strange behavior of sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi,

The root cause of this problem is using a vertical reference option when creating/defining the sketch. It is a bug and we fixed this in NX 11.0. We are sorry for the confusion.

 

Regards, **bleep**