How to offset and extrude text outlines?

[jskinner58]

I have some outlines I imported as svg.  I unfixed them so I can edit them but still have difficulty doing what I want.  Working on two sides of an embossing die set.  For one side I want to extrude a profile that is 0.015" smaller than the outline and attach that to a thick block.  For the other side I want to extrude an outline that is 0.015" bigger than the outline into a block and take away that material.  I am having difficulty knowing the best order of steps to take.  I have the outline of the block and the letters in a file and planned to take a copy of that for the top block and another for the bottom block.  I can't seem to do the offset on the outline but can extrude it.  Then if I offset I get the outline I want but need to delete the first extrusion and move the second back to the original plane.  I have just put two letters on the block for now to work out how to do this.

[Phil.E]

So it sounds like the actual problem here is that you cannot offset the SVG text outlines?

Can you attach your SVG file to this post?

Thanks,

[jskinner58]

I don't have the svg file.  For one thing I deleted a bunch of the things in the file after import to make things simplier to try things.  I am attaching the fusion file.  I added the block and circles on each end in Fusion. 

I am having trouble selecting the outlines to do the offset.  I can push/pull and then do an offset on top of that. 

When selecting the outline of a letter I get several segments but not the entire outline.  I am too new to fusion to know what the issue is or how to group the segments so they all are selected.

There are also a couple of points that show up on the view.  Not sure what that indicates...

[Phil.E]

You should be able to offset the original 'green' lines of your SVG import as one 'loop'. I think the SVG has some problems that are preventing this.

If you open your file and drag some of the sketch lines, you'll find other sketch lines underneath them.

So I would try this:

a) re-import your svg and don't unground anything. Does it offset as one loop? If not can you clean it up in the program it came from?

b) or, just use Sketch text in Fusion to achieve your goal.

The only way I can tell for sure is if you provide the original SVG.

Thanks,

[jskinner58]

I went back to Inkscape and put in one letter and inserted the svg into fusion.  The outline is in green lines.  My other one is blue.  What does the line color indicate?

I offset the letter in the new file.  No problem doing that.  But then how to get rid of the original letter outline?  I deleted the offset symbol to try to unlink the offset from the original but then symbols appeared by every line segment.  Do I have to delete all those?  And the offset and orignal outline now appear to be a bunch of line segments rather than one outline where I can select the whole thing with one click. 

I want to get one outline slightly smaller and one slightly bigger than the original.  How do I reasonably easily do this??

[donsmac]

This will help:

[jskinner58]

Thanks.  I was able to get that far.  I am stuck at the next step of making the extruded size slightly larger or smaller than the original by the offset amount.

[Phil.E]

@jskinner58

First to answer your question, fixed sketch geometry is green, unfixed is blue.

You say:

"I offset the letter in the new file.  No problem doing that.  But then how to get rid of the original letter outline?  I deleted the offset symbol to try to unlink the offset from the original but then symbols appeared by every line segment.  Do I have to delete all those?  And the offset and orignal outline now appear to be a bunch of line segments rather than one outline where I can select the whole thing with one click."

I'm not sure you need to get rid of the original, but if you want to you are on the right track. The little symbols are showing the sketch constraints.

Here is a video showing

1. Make a sketch letter

2. Explode the text

3. Offset inside and outside

4. Extrude inside and outside shapes. (this can be done in any combination, going in any direction)

If you want to use the sketch twice, make it visible after using it once.

Let us know if you have any other questions please.

Thanks,

[jskinner58]

I started over and imported the svg again and everything seems to be working fine this time.  There were a few extra lines that weren't visible in Inkscape (the colors were "no color") that I ended up hunting down and deleting before importing but I tried it with and without those changes and both times things worked as expected.  Not sure what happened on the original one...

[jskinner58]

I spoke too soon.  I was able to generate the outline offsets and fillet the corners of the small letter but on the bigger one it refused to do the fillets with the error "Failed to solve.  Please try revising dimensions or constraints."  I tried drawing two lines  at right angles well away from the letters and putting a fillet in the corner.  I even removed the right angle constraint.  Still got the same error.  Closed F360 and reopened it.  Still the same.  I went back to an earlier version and was able to fillet the top left corner of the n but if I offset outlines in and out 0.015" I was not able to fillet the corners and got the same error message.  Seems like a bug but perhaps not.  Am attaching file with no offsets for n and the one with offsets that doesn't fillet.

[jskinner58]

A work around is to extrude first and then fillet but this still seems like a bug.  I thought it was easier to see the clearances and visualize what I was doing on the sketch for the small letter but that's not such an issue on the larger one.  And in the sketch I could do all the fillets without having to rotate the part view so it's a bit quicker. 

[jeff_strater]

I agree - this seems like a bug in sketch fillet.  We'll take a look at it.  I see no reason why those lines cannot be filleted.  It probably is some remaining issues with the geometry after the offset has been removed.  

And you are correct, the workaround is to do the fillet as a solid fillet.  Personally, I prefer the solid fillet anyway, but I agree, you shouldn't be forced to do it that way.

Jeff Strater (Fusion development)

[jiang_peng]

Hi,

One possible cause of the failure in your design is that after delete offset constraint, there is an illegal tangent constraint in the sketch, please delete it:

We are still investigating why there is a tangent constraint here.

Thanks

[jskinner58]

Here is another issue I have with fillet - see the attached.  Look closely at the small M.  In the center the second curve from the bottom.  The ends don't quite match up with the curves to each side if you look closely.  You can barely see it when zoomed in as much as possible (why can't I zoom further?).  In one model I was able to push the curve down until they intersected and trim the lines but that doesn't seem to work on this one - I can't see enough detail to position and when I try to move it the side curves move with it.  I can delete the center curve, extend the side ones and fillet in the model later but that is a lot of fiddling.  And it is so small I might not have even noticed the issue. 

[jiang_peng]

Could you please attach a snapshot? I checked the small "m" but not able to to find the issue.

Thanks for the help!

[jeff_strater]

Is this the problem that you are referring to?

It seems like there is some missing constraints here - the endpoints of these curves are not coincident.  It's not clear to me whether this geometry was from the imported SVG, or from the offset.  If you can help us understand where this geometry came from, we can look into where it comes from.

To fix it, you can do something like this:

Thanks for point this out, we can continue to investigate this.

To reiterate a point by @Phil.E:  Fusion supports text itself - in sketch.  So, if all you need is text, I would bypass SVG completely.  You are likely to get better results overall.  The SVG path should definitely work, of course.  But, there are fewer steps involved in using text directly.

Jeff

[jskinner58]

That is the issue I was referring to.  I made the outlines by:

Importing font outlines as svg.

Offset those outlines for slightly smaller and slightly larger outline.

Deleted original outline.

Applied fillets to corners of outlines

Given how the fillets were created, I don't see how the problem was in the svg import, or if it was, why F360 didn't show some error.  I think I can supply the file at several points of the process if desired.

I understand F360 has text ability.  But I have modifications to some of the text that I need to import.  It just isn't shown in the samples.  I am trying to take a couple letters through the CAD and CAM process to make sure everything works as expected and make any needed adjustments before I do the whole thing.

I just noticed that I don't have a tangent symbol where fillets meet where there isn't another line segment between them (such as the line below the issue I reported).  I ran into similar issue when I applied fillets to an extruded shape (top of the "n") and they overlapped.  I expected the fillets to be tangent (isn't that the basic idea of a fillet?).  Perhaps this non-tangent behaviour is expected behaviour if the fillets are too big to fit?  I expected this would generate an error. 

It appears that to make sure the lines are tangent  I need to vary the size of the fillets and make sure I have a slight spacing between them?  If I just connect them as in the video and then apply tangent doesn't the radius have to adjust?  I need to keep a minimum radius so it can be machined.

[jeff_strater]

Thanks @jskinner58, for the info.

I agree that sketch text is not sufficient if you need to make modifications.  So, yeah, SVG should work, I agree.

I agree, this does not seem like an SVG import problem.  Offhand, I think this might be a sketch fillet bug.  The bad part is these two lines:

I suspect what happens is that the offset has a very short line in it, and when you go to fillet, that line is actually flipped so that it goes the other way.  That's why you see the kind of "backward tangent" condition with these lines.

If we had the original SVG or even an example with the "M" from this font in it, we could try to figure out what is going wrong with the fillet.

Thanks,

Jeff

[jskinner58]

You gave me some ideas.  I don't have complete history but went back and tried a few things.  I think the end of one fillet ended very close to the end of the line segment and when I did the next fillet it connected to the line rather than the previous fillet.  But it was so small I didn't notice it until later.  I did a couple of pictures to show the inner outline and a fillet that produces a line segment that is reversed.  I made it a bit larger so it can be seen.  Now that I see what happened it probably isn't considered a bug.  I will just have to be careful to not end a fillet very close to an end point.  I think the line could be extended before the fillet to avoid the issue.

[jeff_strater]

Thanks, @jskinner58, I suspect you are right.  I still think that fillet should not generate that geometry, so we'll look into it.  Thanks for the pointers to reproduce it.

Jeff