Re-scaling imported DXF

Ihab

Hi folks,

When I import a DXF file into an OnShape sketch, it currently imports the file as a series of individual lines and points with no constraints. They cannot be treated as a group, and I am unable to add a single driving dimension to re-scale the whole shape.

Is this a new change to OnShape? Am I missing something?

I am aware of the following post on the topic:

https://forum.onshape.com/discussion/16285/reszie-a-dxf-import-file

Ihab

Hm, interesting. I just re-tried this and realized I may be mistaken…. But still, I find the behavior confusing.

Below is a sketch into which I inserted a DXF file. All the sketch elements created as a result are unconstrained.

I added a dimension restricting the distance between two points of the imported elements. This did correctly rescale all the elements.

However, since the elements remain un-constrained, I cannot confidently move them (e.g. to make the entire object coincident with the sketch origin). If I add constraints, they do not constrain the remainder of the DXF elements; instead, the DXF elements are ripped apart from each other.

I can work with this … but … the behavior is counter-intuitive to me.

Ihab

eric_pesty

Your best bet is to use the sketch transform tool to locate something like this:
Box select everything ⇒ transform ⇒ move the transform "anchor" to were you want the origin and drag the whole thing until it snaps to the origin.

Ihab

Got it, thank you! Moving the transform "anchor" does not snap to the DXF geometry so it is an approximate operation, but it certainly solves the problem of having geometry positioned far the heck away somewhere!

Ihab

MDesign

The sketch transform tool can and will snap to any imported dxf entities just like any other entity becuase once imported its no longer a dxf its onshape sketch entities

Ihab

Thanks folks! So I arrived at my next interesting discovery.

In the example below, I have imported a DXF of the "flower" shape and added a driving dimension, which correctly scales the entire shape to 18 inches width.

When the dimension (circled in red) is a configuration variable, however, this scheme does not work. In particular:

• Changing the default value of the configuration variable has no effect on my model; and
• The changes sometimes cause my DXF geometry to be "ripped apart".

So as best I can tell, the "resize DXF with a driving dimension" technique does not compose with the other parametric features of OnShape.

Can anyone confirm, or tell me what I'm doing wrong?

I was hoping to create a configurable assembly containing all the parts of my logo, that I could paste into any design at any size of my choosing. Right now I am just copying and pasting new versions for each size I'm going to need. Not super parametric, but it gets me unblocked.

Ihab

MDesign

Are you creating any 3d geometry from these sketches? If so I'd highly recommend simplifing the sketch's and driving your paremetrics from there and the utilizing patterns where applicable.

Ihab

Got it, thank you! Yes I am creating 3D geometry, and … it is for a logo that I am creating in large size using metal or wood pieces. The exact shape of the logo is determined by the genius of the graphic designers and it is not for me, a mere engineer who just hacks CAD and bangs screws, to simplify or modify it! :)

But thank you!

Ihab

MDesign

Simplify to at least this would be my recommendation

eric_pesty

The best way to deal with this is to create a "surface" out of your imported sketch. You can use the offset surface with zero offset to create it, then create a composite part as these are "dis-jointed". Then you can derive that into your design part studio and scale/transform it as you want.
A flat surface can be used just like a sketch region for any kind of feature like extrude, thicken, etc…