Engraved text -well, awful

[sjj530]

I'm trying to engrave some text on a flat surface.  Should be simple, but the results are very disappointing.   In the photo below you can see the letters are out-of-round, straggly, and just plain bad.     I'm sure it must be operator error.   I have to be defining the toolpath incorrectly but my research hasn't suggested an answer. 

I ran the same text, same size, same bit, same depth, using Inkscape > F-Engrave instead of Fusion and the results were much better. I'm pretty sure, therefore, that the problem is not in the CNC, the bit, or the workholding.  

Any suggestions would be greatly appreciated.  Thanks!

[gabriele.esposito]

Hi @sjj530, I have seen how you generated the text, maybe you could try changing the font, I attach the project with an example of Engrave toolpath.

Also try to see this article:

How to engrave single line text in Fusion 360

[DarthBane55]

With all due respect sir, are companies now supposed to change the font of their logos because Fusion can't engrave some fonts properly?  That was not a very helpful answer for OP, I feel for him... 

I looked but sorry I cannot help on this.  Hopefully someone makes it work with proper solution.  My answer also not very helpful, I know that...  

[HughesTooling]

@sjj530  Can you edit your sketches and explode the text to curves then re-share the design please. Because I don't have the font you used installed on my PC, Fusion changes it to Arial so can't help.

[HughesTooling]

@sjj530  Looking at the F-Engrave page here, did you use V-Carve or B-Carving? B-Carving looks interesting and might give a different look to Fusion's Engrave option.

Mark

[sjj530]

Thanks for all the feedback!

gabriele.esposito - I could change the font.  I see the article you referenced used an *.shx font.  I guess those are an Autodesk-specific font.  I'll try it, to see if it works better.    Unfortunately none of the shx fonts available give me the particular look I want. 

DarthBane55 -- I agree, I can't believe that Fusion 360 cannot support engraving multiple font types.  I did try exploding the text, but the results were no better.  And the engraving problem isn't just with the text, although I left that out in the original post.   Even simple curves look bad -- you can see the jaggedness of the curve in the  upper-left of the first picture.   Now that is a smooth curve in the sketch, but was milled jaggedly.  It was what made me first assume the problem was in the CNC -- but that turned out not to be the case. 

HughesTooling  -- I have attached a version with the exploded letters.  In F-engrave, I used V-carve instead of B-carve because this art deco-ish font has serifs, which can only be engraved with a v-bit.

[sjj530]

Now I'm wondering if the surface speed of the bit could possibly be a factor. The F-engrave carving moved considerably faster than the Fusion 360 carving, although the DOC was the same.
This seems a very difficult issue for what is basically a very simple task. People must be using Fusion 360 to carve text hundreds of times a day. I must be missing something simple.

[HughesTooling]

The simulation in Fusion looks quite good so I think it's just a case of getting the correct feed rate.

One thing I did notice is in areas where sections of the letters cross the tool plunges a lot deeper, did you set a max depth in the other program you used?

I've highlighted some of the areas I think might cause a problem.

Mark

[HughesTooling]

Just adding to the above.

Below you can see most of the letter is machined at around -1.25mm but at the intersections it going down to 1.85mm. If the feed's a bit too high this might cause problems.

The only problem is if I set the max depth in the engrave op to 1.25mm it doesn't clear all the material at the intersections. Can you share the code from F-Engrave? You might need to change the extension of the file to txt.

Below you can see the difference if you set the depth to -1.25mm

[engineguy]

@sjj530 

Hmmm, bit of an odd one this, you may have already looked at a couple of things that I always look at when doing custom Fonts are the "Tolerance" and also the "Sharp Corner Angle", the latter one is especially important I have found as it changes the way the toolpath is generated considerably.

See the two images below, the first one is with the toolpath generated using the default 165 Degrees and the second one using a setting of 90 Degrees, reason for the large difference in values is just to show more clearly how the engraving changes, the 90 Degrees is much smoother, no corners, may be of some help to you, I don`t know if you have already looked at this.

P.S. I don`t seem to get any extra depths, all at the 1.25 DOC unless climbing the corners ???

P.P.S. The above was done using you original unexploded file.

[sjj530]

Thanks, Mark, for continuing to look into this little problem.   I understand your point about the bit moving lower at the letter vertices.    I think these are points where the strokes of the letters -- including the serifs -- intersect.

I don't think that is the source of the problem, though.  Referring to the original picture I posted, you can see the that the irregularity in the "O" letter can't be ascribed to the bit dipping lower at the vertices, since there aren't any.  And for the "R" character, the straggliness occurs along the front vertical line of the 'R" - that is, where the bit should be moving at a constant Z-height.

Just to simplify the problem, I created two sample gcode files using just the text "Morgan".   The first was created using Fusion, typeface AR BONNE, rotated -60 degrees, 2D Engrave, max depth -3 mm,  using a 0.25" 90 degree bit. 

The second was created using Inkcape, same typeface, same rotation, and the gcode was created using F-Engrave with the same bit, and also set to a maximum depth of -3 mm.

I haven't dived into the gcode yet, but I noticed the F-Engrave file is more than twice as large as the Fusion 360 file.  Presumably that means the F-Engrave version is doing more milling, which certainly appears to be the case when the jobs are actually run. 

[sjj530]

Thanks for the suggestion, engineguy!   I had not considered modifying either of those two settings.  I will look into it -- maybe that will be the fix! 

[HughesTooling]

Looking at the 2 programs together the biggest difference is  F-Engrave is going around the letters at 2 heights. So I think the single cut to depth in Fusion is too much for your machine's rigidity.

In the image below the green is F-Engrave and blue is Fusion, apart from a small size difference they are very similar. Just found another difference, F-Engrave goes around each letter twice at each level so it looks like it goes around each letter 4 times.

[HughesTooling · Accepted solution]

You can achieve something similar in Fusion if you set a maximum stepdown and then if that's not good enough you could repeat the engrave op just at the max depth as a spring cut.

See attached file, the second engrave op is just a copy of the first but just a single depth. Also your spindle speed in the F-Engrave file was only 3,000 and 18,000 in Fusion

[sjj530]

Thanks, Mark!  I think you've found the answer.   Executing at multiple depths, followed by a spring pass gives the best results. 

Slightly off-topic - regarding the differences between F-Engrave and Fusion.  I noticed that in addition to running multiple passes, F-engrave also moves the bit both clockwise and CCW on each letter.   That may make a difference.    Unfortunately, I can't replicate that motion in Fusion, as Fusion's Engrave toolpath does not allow the option to change the direction of the bit.   F-Engrave also spends more time than Fusion does on the corners and serifs.   Overall, the quality of the result is still better in F-Engrave than Fusion. 

Thanks for all your help!

[DarthBane55]

@sjj530 

I am no expert in engraving, but I find strange to run the bit CCW, the cutting edge is surely only on 1 side... so maybe it sort of polishes the edge when it does CCW, interesting.  You can do that in Fusion too... Copy the tool and set the rotation CCW on the copy, then copy the toolpath, pick that new tool.  It will run the same toolpath but in CCW rotation of the tool.  You probably can remove the multiple depths of cuts and keep only the last depth for that pass.

[HughesTooling]

---

@DarthBane55 wrote:

@sjj530 

I am no expert in engraving, but I find strange to run the bit CCW, the cutting edge is surely only on 1 side... so maybe it sort of polishes the edge when it does CCW, interesting.  You can do that in Fusion too... Copy the tool and set the rotation CCW on the copy, then copy the toolpath, pick that new tool.  It will run the same toolpath but in CCW rotation of the tool.  You probably can remove the multiple depths of cuts and keep only the last depth for that pass.

---

The tool doesn't run CCW it's the direction around each letter, F-Carve does a pass in one direction then goes back around at the same level in the opposite direction. Fusion doesn't do this and I doubt it's something they'd add as it's not needed on a rigid machine. I'd guess F-Carve has been designed for the DIY market where multiple passes in both directions are needed to make up for the machines.

Mark

[DarthBane55]

@HughesTooling 

Ah that makes more sense!  so in Fusion we can't say "1 way" or "other way" for engraving?  Too bad I suppose, for some users. Thanks for clarifying !

[HughesTooling]

@DarthBane55 Yes that's it and now you've mentioned One Way and Other Way I think that would be quite useful. I usually engrave copper and it would be helpful if the burr was pushed to the outside of the letter (CCW around the letter I think). @seth.madore Is that something that could be put on the wish list, cut CW or CCW?

Thanks Mark