Translate or move Curves/ Lines?

[Hockeyguy]

Hi,

Is there a way to translate or move a line in a sketch?

Example move a line the Z axis + or -?

Thank you

 

[jerry1423]

as long as it's not constrained you should be able to move it using: edit > Move Object

 

[Xwheelguy]

To expand a little more, you'd have to be in the sketch mode (sketcher application) to do so.

Outside of the sketch, (modeling application), it would probably be treated as a feature, and your best bet might be to redefine the datums associated to the sketch (reattach the sketch to a different set of datums). There's probably more than one way to do this.

Sketches, regardless of their TRUE plane location are typically XY (flat, no Z) when the sketch mode is activated....or horizontal/vertical...you might want to elaborate a bit to avoid any confusion.

Tim Flater
Senior Designer

 

[JohnRBaker]

Whether it's constrained within the Sketch or not, a line created inside the Sketcher will lie on the X-Y Plane of the Sketch and cannot be moved off that plane. Even before we replaced most of the Transform functions with Move Object, you could NOT move a Sketch curve in the Z-direction, that is off the plane of the Sketch.

Once outside the Sketcher, a entire Sketch is treated as single object by other NX function such as Transform in the past and Move Object today.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[jerry1423]

oh you are right, it (the curve) can only be moved in the x and y planes. You need to move the plane itself if you want it to move in the z axis.

 

[JohnRBaker]

The best that you can do is to create a non-feature-based curve (dumb curve) outside the Sketcher which does NOT lie on the sketch plane and then go back into the existing Sketch and add this curve to the Sketch. Now the only thing that you can do is control the location of the end points of the curve, AS PROJECTED ONTO THE PLANE OF THE SKETCH, but NOT the 'Z' location (height) of those end points.

And while this curve is technically part of the Sketch, it may be problematic if you later attempt to use this sketch as a profile for some Modeling operation like Extrude or as a reference curve in a Surface creation operation, if you include it in the selection of the Sketch for the Modeling operation.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[kerbosos]

I just want to add that any sketch geometry based on projected curves CAN be deleted (although it generates a system warning dialog) after that particular sketch element is created.

I use this method all the time when aligning a though hole for joining multiple parts that need to be match drilled on assembly.

 

[jerry1423]

In a situation like yours, where you have a hole in one part (part A) and need to determine the location of that hole in a mating part (part B) - Is (in the assembly) make the component Part B the work part, then extract the hole edge from Part A
Insert > curve from bodies > extract . . .
The hole edge will then show up as a curve in Part B and you can create your hole based off that.

You can also just make Part B your work part in the assembly and create the hole in there.

 

[JohnRBaker]

But if it's true that what you're creating are drilling operations which will be done AT assembly, then you DON'T want these holes to end up in the detailed part models. Instead you should be looking at creating something like a tool solid in the context of the assembly representing the volume of space needed to be removed, resulting in a 'drilled' hole. This can be done by using...

Insert -> Combine -> Assembly Cut...

...where you can perform of the modeling operations, subtracting the tool solid from the ASSEMBLY model, AT the assembly level thus duplicating what the realworld workflow would actually be. If you go to the Help files and look at the 'How to" section of the Assembly Cut documentation there is an example ther similar to what you're decribing.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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