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Problem with Import "data from file"

JCAD

New member
I have a sketched profile which is my protrusion from one part that I need to use in another part, I save this sketch in sketcher , when I use Data from file in my new part, the sketch appears okay in sketcher, I then position the sketch with the move handles I then select the scale and click the tick check mark. This is when I have the problem..... The top part of the sketch is fine, but the bottom part goes all weird and out of shape, I can only imagine that it has something to do with the references used for the sketch??? what is the best method when using data from file for duplicating a profile to be used as a sketch in another part?
 

dougr

New member
The problem is that some of your dimensions are to references outside of your sketch (datum-planes, edges, vertices etc) when you save your sketch.



These dimensions cannot be saved in an sec file (think about it) so intent manager is free to make assumptions about the geometry when you go to place it - as you found out...



To get round this I usually place a vertical & horiizontal centerline to dimension off in sketches:



View attachment 330



The centerlines can then be aligned or dimensioned to external features to place the section.
 

JCAD

New member
Cheers Doug, managed to get it to work, the sketch i was trying to save was quite complex and had about 80 dimensions, I created horizontal and vertical centrelines and removed the default datum sketch references, I then made sure that all my dimensions were strong before I saved the sketch. I was then able to import my sketch without it going out of shape.............. because i went into redefine on the original part is it good practice to cancel out of the original part sketch without saving the changes to the refs, because the original sketch would then not reference to any local part geometry, it would only reference to centrelines wouldn't this affect my design intent???
 

dougr

New member
is it good practice to cancel out of the original part sketch



I'd say not just to preserve your work (I would save it) but it's up to you.



I'm in the habit of placing centerlines in every sketch now just so I can reuse them in this manner..



Also enables you to prepare sketches offline in sketch mode.
 

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