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NX 11 Reuse Sketch

Experimenter
Experimenter

Hello!

 

I would like to use a sketch in NX 11 in one part several times and when I change something in one of them, all of them should be changed.

 

So i can copy and paste the sketch, but than i just can make the sketches associative with the function "connect to the Original" (expressions are connected from the first sketch to the copied one). That's nice BUT: When I add another element (for example a line) in the first sketch, I would like to see the line in the second one, too.

I think using the "reuse Library" or "UDFs" also can't solve this problem.

I also tried "Pattern Geometry", but there I can't fix the two sketches on different pathes, I think.

 

Isn't there a Possibility to create a "Mothersketch", which can be inserted in my part file several times - e. g. each on a different path? And when i change something in this "Mothersketch" in each sketch the change is also edited?

 

I hope there is a solution to my problem.

 

Thanks a lot and bye

Carsten

6 REPLIES

Re: NX 11 Reuse Sketch

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Create the sketch in a separate part

Assemble the part in as many times & positions as needed to the actual "piece-part"

(if needed) WAVE link the sketch into the "piece-part"

extrude/revolve/whatever as needed.

 

Use PLIST_IGNORE attribute (or other techniques) to prevent it from showing up in parts lists

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: NX 11 Reuse Sketch

Experimenter
Experimenter

Hello Ken,

 

thank you very much for your answer. I had to do work for another project, so I couldn’t answer you earlier…..

Meanwhile I had time to try out your solution but I still have problems to manage the issue. Here a few additional information to my project: I have to create a railway tunnel model with two axes (wich lead to one tunnel later) in which I would like to insert the cross section of the cut-and-cover-tunnel (rectangle cross-section) along the axes (pathes) one time each. When I add another a line or similar I would like to have them automatically in all sketches.

 

So according to your solution I created a part-file with the sketch of a cross-section in and attached it to a path (a “dummy line”). This sketch I assembled two times in the other part with assembly constraints, wave linked it and tried to create an extrusion with the command “Swept” and “Variational Sweep”. But it didn't work and I had to create another Sketch, in wich I projected the lines of the cross-section-sketch. If I don’t do this I can’t create the Extrusions. Here NX shows alerts:

Swept: “Unable to create single curve from a profile having multiple loops.”

Variational Sweep: “The section containes one or more curves outside a single sketch on path. Select curves from one sketch on path for the entire section.”

With the Sketch with the projected lines I can do the Sweep with "swept".

 

So my problem is just solved partly, because when I add lines to the cross-section-part they will be in the assembled sketches, too. But I have to project them additionally into the sketch, which I sweep at long last.

 

Have I done it like you suggested or do I have to do something different...?

 

I hope you can help me further another time.

 

Thanks in advance!

 

Carsten

___________________________________________________________________________________________

 

Supplement to my answer:

1. With "swept" I don't have to make the sketch with the projected lines but i can't create a Body with a hole (see text of the alert above).

2. When I use the command "Sweep along guide" it seems to work without alerts.

Re: NX 11 Reuse Sketch

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

A couple suggestions...

1) Convert all the lines/curves that you do NOT want to extrude to "reference" curves.

2) Pay attention to the "selection intent" toolbar when selecting curves to extrude (single curve/connected curves/tangent curves/ feature curves/etc.) to make it easier to select just the curves you want to extrude.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: NX 11 Reuse Sketch

Experimenter
Experimenter

to 1)

That doesnt't seem to change something for the extrusions with "swept" and "variational sweep".

 

to 2)

I paid attention to this function. So I already have selected the correct lines for the extrusions.

 

I think the problem are the two connected curves that run parallel so I can't select them for the extrusion.

 

But I'm thinking with selecting "Sweep along guide" for my extrusions, I can solve the problem.

 

So thank you for the solution with the sketch in the separate part-file - I will test respectively study the whole topic for a while.

Re: NX 11 Reuse Sketch

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Carsten -

At this point, if you need further help, we may need a (simplified?) example of what you are trying to do, to understand the issues you are encountering.

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: NX 11 Reuse Sketch

Experimenter
Experimenter

Hello Ken!

We had so many thoughts about the topic, that I would like to try going deeper by myself first. Maybe you already solved the problem.

Thank You so far!

Greetings

Carsten