Scaling a project
@dmack3396 - it seems to work for me. You want to just scale the body, I think, so I would select that in the browser. You can choose a different point to scale about if you want, but the default seems to be OK:
Jeff Strater
Engineering Director
Right click the sketch in the timeline and select edit. When in sketch edit mode select scale from the sketch menu or if you have the new UI from the sketch modify menu. It will take a while to select, select a base point then enter a scale of 0.8 should scale dont to about 24".
Mark
Mark Hughes
Owner, Hughes Tooling
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sorry - I was outside doing some spring chores. I seem to have been caught in the dreaded forum spam filter - somehow my post got taken down...
Anyway, I'll try again. First of all, I would scale the body, not the sketch. That's what my screencast below shows. There is really no need to scale the sketch, other than maybe wanting the sketch to match the result. So, option 1 is to just scale the body. If you want to scale the sketch, the reason you don't see the scale factor text entry box is because you have not yet chosen a center point for the scale. This is an inconsistency between body scale and sketch scale - body scale chooses one for you, sketch scale does not. Once you pick a point (the sketch origin is as good as any), you should see the scale factor text box.
Jeff Strater
Engineering Director
@Anonymous wrote:
I don't mean to sound like a smart ass, but I know how to scale objects. In the first email I stated that box does not come up to type in the size to scale to. I can click and have as many points as I want. The little box on the side keeps saying how many points I have selected but the box does not pop up to type in the scale.
The reason you're not able to enter a scale is you need to set a base point. Where it says point on the dialog you need to highlight and pick a point. Not sure why but the sketch scale doesn't automatically select a point like the solid scale does, that said the auto select always selects the wrong point so perhaps it shouldn't pick a point either.
Mark
Mark Hughes
Owner, Hughes Tooling
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@jeff_strater wrote:
Anyway, I'll try again. First of all, I would scale the body, not the sketch. That's what my screencast below shows. There is really no need to scale the sketch, other than maybe wanting the sketch to match the result.
@jeff_strater I think @Anonymous might want to machine this in the CAM workspace so the sketch lines might be useful, especially the open curves not in the extruded model.
Mark
Mark Hughes
Owner, Hughes Tooling
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good point, @HughesTooling . You should be able to scale the sketch just fine. There are a lot of entities in this sketch, so it is a bit slow, but it does scale OK.
Jeff Strater
Engineering Director
@Anonymous - That's interesting. The error is misleading, at best, and my guess is that it is kind of a "throw up our hands/default error" when we don't know what else to report.
In my opinion, this illustrates the hazards of working with imported (presumably SVG) sketches, and scaling a sketch. Imported geometry does not have constraints that hold it together, so under a scale operation, you can get gaps or other anomalies in the resulting geometry. Also, this sketch has about 5000 entities in it, which makes working with it in sketch really challenging. So, I'll go back to my original recommendation: Just scale the body. If you need sketch lines for doing CAM toolpath operations, I'd just create a second sketch on the resulting top face of the Extrude.
But, I can offer a bit more insight into what I found looking at this sketch after the scale. Using a version of the "divide and conquer" technique here: find-break-in-sketch-geometry I was able to find the area that has the problem:
Then, further refining this, to this small area:
zooming in close, you can see some problem sketch geometry:
If I deleted all those extra curves, I can then extrude OK:
However, I did find another problem with your scaled sketch - the main internal profile of the Marlin is no longer recognized after the scale:
using the same divide and conquer technique, I found another problem:
I did the same basic thing to repair the sketch in this area, and then can extrude the entire shape OK:
I've attached this repaired version to this post.
I guess my recommendations would be:
- Be careful, or avoid if you can. using imported SVG or DXF data - there can be a lot of curves, which makes Fusion's sketcher crazy, and if scaled, can result in these types of problems. Systems which create SVGs are notoriously imprecise, and generate a LOT of curves. Fine for doing 2D art, but not so great for a parametric CAD system. If, for instance, you ever want to try to fillet the termination edges of this extrude, I would not predict success.
- I still would prefer to scale the body, not the sketch
Jeff Strater
Engineering Director