Old World Map - A learning experience

[jteneyck]

I bought a file off Etsy to make this old world map on my CNC. 



I created three toolpaths to carve it, a roughing toolpath, and two finishing toolpaths, one with a 1/8" tapered ballnose endmill, and the final one with a 0.5 mm tapered ballnose endmill.  For finishing toolpaths you typically use a stepove of 4 to 8%.  Stepover is how far the bit moves with each consecutive pass.  So 8% with a 0.5 mm bit means the bit moves 0.04 mm with each pass.  To save machining time I set the final toolpath with an 8% stepover.  It still took 35 hours for that step, and over 50 hours for the three toolpaths. The rendering looked great so I thought it would look good after machining.  Not so.  Here's what it actually looks like.



It looks pretty good, but it's clear a lot of details are missing.  Compare this closeup with the top left corner of the model rendering. 


 
It may not be obvious, but some writing is missing on both the hemisphere and surrounding border, and the lines of longitude should be more defined.  But where did I go wrong?  I looked at the rendering again and it looked great.  Finally, I realized that the rendering I was looking at was the one you see above, the one provided in the Etsy file.  Only when I looked at the final toolpath separately did I see the problem.  



Learned a lesson there.  Always look at the individual toolpaths.  So, by reducing the stepover from 8 to 4% the final toolpath now looks like this.



Holy cow what an improvement.  You can see how many more details have been added.  But at a major time penalty.  The total machine time now is 147 hours.  Oh boy, I may have to reconsider getting a spindle sooner than I intended.  Stay tuned.  

John

[J-W-P]

147 hours, wow.
How big is the piece?
What are your feed rates?

[MKepke]

147 hours, wow.
How big is the piece?
What are your feed rates?

Also my thinking: reduce your step over but look at increasing your feed rates, rapids and using some form of intelligent REST machining if you aren’t already (with simple 3D rough and finish toolpaths, the finish tool path will still amble over 100% of the surface even if some areas won’t benefit/be cut).

-Mark

[jteneyck]

147 hours, wow.
How big is the piece?
What are your feed rates?

The carve area is about 14 x 26.  The roughing pass takes 7 hours.  It's done with a 1/4" ball nose endmill running at 120 ipm, 40 ipm plunge rate, and 40% stepover.  The finish clearing pass takes over 80 hours and is done with a 1.5 mm tapered ball nose endmill running at 75 ipm and 75 ipm plunge rate, with a 4% stepover and mid level rest machining of 0.001".  The final finishing pass is done with a 0.5 mm tapered ball nose endmill running at 36 ipm and 36 ipm plunge rate, with a 4% stepover.  It takes 68 hours, so I'm up to almost 160 hours (estimated) now.  

What would you change?  This seems ridiculously long, but I've already pushed the speeds for the tapered bits well beyond the values recommended by the manufacturer.   

John

[J-W-P]

I've not done any 3d projects that large and intricate, but the estimated hours seems crazy. Is the time estimate from vectric toolpath summary or onefinity after it has processed the gcode?

For your roughing plunge rate I think you could bump that up to at least 60-70 but that won't make much difference.

Maybe use a larger tapered ball nose (1/8") at 8%, ~75-100 ipm feed for your first finish pass, then the 1.5mm for the second finish pass

I'm fairly new to vectric/onefinity myself, so my suggestions should be taken lightly

[jteneyck]

I've not done any 3d projects that large and intricate, but the estimated hours seems crazy. Is the time estimate from vectric toolpath summary or onefinity after it has processed the gcode?

For your roughing plunge rate I think you could bump that up to at least 60-70 but that won't make much difference.

Maybe use a larger tapered ball nose (1/8") at 8%, ~75-100 ipm feed for your first finish pass, then the 1.5mm for the second finish pass

I'm fairly new to vectric/onefinity myself, so my suggestions should be taken lightly

Thanks for the feedback.  Changing the plunge rate on the roughing pass isn't going to make much difference.  I used a 1/8" tapered ball nose endmill with a 20% stepover to get what you see in the photo.  The time estimates are based on what the OneFinity shows from the toolpaths created in V-Carve.  Then I used the scale factor in V-Carve to get approx. the same times, at least the total time, for new toolpath options.  I won't know for sure what the times are until I load it in the OneFinity.   

OK, I reran it with the 1/8" TBEN at 4% stepover, followed by the 1.5 mm TBNE, also at 4%.  By golly, it looks pretty good, and the total time is down to 81 hours, about 32 hours for the 1/8" and 42 hours for the 1.5 mm.  I can try and see how it looks.  I'm using the same carving, just going deeper each time, so it's not like I'm wasting new wood.  There's no need to run the roughing path again, either, since I'm only going about 0.020" deeper.   Thanks, I may give it a go with the 1/8" bit tomorrow.  These projects are learning experiences, and there's a lot to learn.  

John

[MKepke]

A couple thoughts here:

1 - you want to use the largest diameter tooling you can because this gets you relatively smaller ridges left after stepovers. So ask yourself if your STL really has details that call for a 0.5mm (radius or diameter?) bit, or even e.g. a 1.5mm bit?

2 - If the STL's areas needing fine detail are isolated, this is where you can use selective REST machining to limit the fine tooling to just those areas.

3. there's a point of rapidly diminishing returns for increasing step-over below about 10%. Below that, machining time goes up faster than surface finish increases.

4 - related to the above, you might be able to get a better surface finish for less machining time by changing your toolpath direction in some areas. Climb cut with the grain, run your toolpaths aligned to the direction of the STL's features.

More explanation of some of these tips here:
https://www.cnccookbook.com/cnc-stepover/

-Mark

[jteneyck]

A couple thoughts here:

1 - you want to use the largest diameter tooling you can because this gets you relatively smaller ridges left after stepovers.  So ask yourself if your STL really has details that call for a 0.5mm (radius or diameter?) bit, or even e.g. a 1.5mm bit?

2 - If the STL's areas needing fine detail are isolated, this is where you can use selective REST machining to limit the fine tooling to just those areas.

3. there's a point of rapidly diminishing returns for increasing step-over below about 10%.  Below that, machining time goes up faster than surface finish increases.

4 - related to the above, you might be able to get a better surface finish for less machining time by changing your toolpath direction in some areas.  Climb cut with the grain, run your toolpaths aligned to the direction of the STL's features.

More explanation of some of these tips here:
https://www.cnccookbook.com/cnc-stepover/

-Mark

Thanks for the tips and advice, Mark.  I've driven myself nuts looking at possible combinations.  The rendering shows areas where even a 1.5 mm bit isn't fine enough.  I thought I ordered a 1.0 mm bit, but it turned out to be 0.5 mm so I used it.  With an 8% stepover it still missed a lot of details.  That only became obvious when I looked at the finishing toolpath separately.  Or maybe it's tied up with the rest machining, which I admit I don't understand very well.  Thanks for the link, I'll take a look at it.  

I am using different machining strategies with the different bits.  With the larger finishing bit I'm using a raster profile, with the smaller bit an offset profile.  

John

[Juss1]

Thanks for the tips and advice, Mark.  I've driven myself nuts looking at possible combinations.  The rendering shows areas where even a 1.5 mm bit isn't fine enough.  I thought I ordered a 1.0 mm bit, but it turned out to be 0.5 mm so I used it.  With an 8% stepover it still missed a lot of details.  That only became obvious when I looked at the finishing toolpath separately.  Or maybe it's tied up with the rest machining, which I admit I don't understand very well.  Thanks for the link, I'll take a look at it.  

I am using different machining strategies with the different bits.  With the larger finishing bit I'm using a raster profile, with the smaller bit an offset profile.  

John

I've only done 2 3D carvings so take my advice for what it's worth.  But I didn't find using 2 finishing tool paths to improve the result.  I did a roughing pass with a 1/4" ball nose and then finishing with 1/16" tapered ball nose.  Initially I had the finishing stepover at 8% and was definitely not satisfied with the result.  I cut it in half and it looked amazing.   It also took twice as long

[FrankAtl]

This is a great thread. I've done numerous motion control systems in the industrial world but just recently got into CNC woodworking so I'm learning a lot from this discussion. Thanks for sharing your experience John!