Company logo on parts (and drawing)

[LOLA-Christian]

Hi guys,
I am trying to get our companys logo on my parts so I can include them in the drawings as well. I have created the logo as a separate part, and saved the sketch (which I reuse on other parts).
Here is my problem: when I have a new part where I want the logo, I make a new sketch, import the previous made sketch, and rescale to fit the new part.
Everything works fine, but then I would like to move or rescale the feature.
Rescale works fine, but not moving.
The letters start to be of different size and all looks terrible....


Any ideas of how I should do it instead?


(using WF3)


Regards
/Christian

 

[mgnt8]

Save it as a STEP or neutral. Then in your new part you can create a coordinate system where you want the logo located & place it there.

 

[TonyJager]

How about if you save the sketch/feature as a UDF?


It almost sounds like that when you import/use a sketch your 'leading dim' are not placing correct. I always made sure that when I saved a sketch I always have a coord in the sketch a dim all the geometry from that. So when you do import/use the sketch you should be able to place your sketchusing the coord, rather then possible from any of the sketcher entities.





Regards





Tony

 

[shankar_me]

Hi,


Go for Insert > Shared data > Merge/Inheritance.


Regards,
Shankar

 

[pjw]

You need to be using sketch level relations to control ALL dimensions in your logo sketch. For example, use a given dimension as a base dimension and normalise all the other dimensions to this dimension for your relations. For example:


Your logo width is 2" wide


Your text is 0.15" high.


You want to maintain all aspect ratios so you write in your sketch level relations:


text height = logo x 0.075.


If you alter the logo width outside of sketcher, the text height updates accordingly. You need to make sure your logo is fully constrained and dimensioned and use the reations to ensure that you only have ONE driving dimension for the whole logo. Dimensions CANNOT change whilst dragging your sketch around because they are now forced dimensions. Just be sure to lock your driving dimension first.


Phil
Edited by: pjw

 

[LOLA-Christian]

Thanks all for the comments, as a "seldom-user" it is a bit difficult to manage this rather complex tool.
Anyway, I managed to solve it with the clue from TonyJager,
and after update of the sketch with an eye of all dimension and
then save the sketch, I was able to reuse it.