Sketch display in drawings 1

[Mandrake22]

I have trouble with sketches in drawings. I have made a graphic overlay for a control panel. This overlay has a lot of extruded text. I have created construction line sketches to aid in the alignment of the text. When I make a DXF export of the overlay (geometry only, no graphics) so it can be laser or water jet cut, the text guide sketches appear. Needless to say, I don't want the cutting machine to follow my guide sketches.

If I suppress these sketches, the text and even some of the features go away as well. No amount of hiding of sketches makes a difference.

I would prefer not to fix the text features and suppress the guide lines.

On a related note, is it possible to force SWX to not display sketches when the drawing is first opened. I always have to turn the sketches off when re-opening any drawing.

 

[SBaugh]

Are you actually talking about Parts instead of drawings?

Because you can really only make one huge amount of sketch lines on a drawing. In a Part you can make a bunch of sketches with minimal amount of sketch lines.

Anyway...

This overlay has a lot of extruded text. I have created construction line sketches to aid in the alignment of the text. When I make a DXF export of the overlay (geometry only, no graphics) so it can be laser or water jet cut, the text guide sketches appear. Needless to say, I don't want the cutting machine to follow my guide sketches.

Try suppressing the features you don't want to export. If that doesn't work, try make 2 copies of the file and delete the items you don't want to export. then Export out what you need.

If I suppress these sketches, the text and even some of the features go away as well. No amount of hiding of sketches makes a difference.

Well that is because you have child dependency going on. If you suppress the sketch well the feature can't be created so the feature is suppressed with it. (Works opposite if you suppress the feature. The Sketch wouldn't suppress then.) The reason some of the other features go away is probably because you used a face to start a sketch which now you have associated that face to that sketch. So if you suppress that parent sketch or feature ALL relations to that sketch or face will be suppressed along with it.

I would prefer not to fix the text features and suppress the guide lines.

If the Guide lines are in a sketch with your geometry then your screwed. Because you can only suppress sketches and not individual lines. You can make a speical sketch that contains nothing but guide lines. You would show this sketch and you can use it for reference or you could use it to guide your geometry. (see my Hanger.zip at my website. I did just what we are talking about here)

On a related note, is it possible to force SWX to not display sketches when the drawing is first opened. I always have to turn the sketches off when re-opening any drawing.

Yes! You click on View and uncheck sketches and save it. After that if you want to hide or see your sketches you have to RMB the sketch in the FM and click hide or show.

Best Regards, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help*

 

[Mandrake22]

Scott,

The sketches are in the part but the problem is with the drawing.

My guide sketches (in the part) are not part of the text sketches. The anchor points of the text are mated coincident to the guide sketch lines and dimensioned to other edges of the part.

I know how to turn off sketches in the drawing but when I save with sketches off and re-open the drawing the darn things are back in all their glory!

 

[meintsi]

You have to hide the sketch lines in your part files for them to stay hidden in your drawing. I just went though this with parts I didn't create.

Go to TOOLS/OPTIONS/FEATURE MANAGER and turn on "scroll selected items into view". Then when you click on an offending item (sketch line) in the drawing, the highlighted part in the feature manager will tell you

1.Which part of the assembly or
2.Which feature in the part (if the part's tree is expanded)

is generating the offending line in your drawing.





Remember...
"If you don't use your head,
your going to have to use your feet."

 

[Mandrake22]

meintsi,

Thanks for the suggestion, but my settings are that way now.
The offending sketches are hidden in the part. Right clicking on them in the feature manager has a "show sketch" selection. View, Sketches is turned off in the main menu.

If it makes any difference, I am runnint 2001+, SP0.0.

 

[SBaugh]

Well upgrade to SP3 at least and try it. If it continues the way your describing, could you send me the files and I'll give them a try here?

Maybe if I see the problem in all their glory, I can give you a better answer.

Regards, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help*

 

[Stoker]

What you are asking for can be accomplished by using a derived part. Create your overlay using the guide sketches in the current manner. Then, create a derived part from the overlay. Your drawing should of course reference the derived part. You cannot access the child sketches in the derived part, so they will not export with the dxf.