Vcarve time estimate

Perhaps I was thrown by the time lapse, but how long should I expect v-carving to take? I was setting up the first job, and between text and a line-art image CC is estimating over 9 hrs. I used the standard settings for #302 60deg Vee.

For scale, the plaque is 14x17", 124 words, text heights ranges from 0.2 - 0.4 inches. (As an aside, how small a text height can I reasonably do?)

9 hrs is only the v-bit time. It doesn’t include surfacing or cutting out the outline.

New at this, thanks for any help,
Adam

In what material?

Post the file?

few things… what did you set the retract height to ? That and the plunge speed are key drivers for long cutting times?

2 Likes

is all the text the same height/thickness?

Default values for v-bit: 35 ipm feedrate, 12ipm plunge rate, .080 depth of cut per pass. Material is Basswood. Retract height is .050".

The text is all the same height / thickness. The line-art has areas that are wider than the text.

2 main questions: What would you expect for a v-engraving this size and how small is it feasible to do a font in terms of letter height (I could make the plaque smaller, but I’m afraid the words wouldn’t be readable).

In Basswood you should be able to move quite a bit faster than that.

Min. V engraving size depends on the angle of the V endmill, the runout on the spindle, and the material one is cutting in.

I’d suggest some test cuts in scrap.

Monkeying with settings to see what changes the estimate, it looks like the plunge-rate is the biggest lever I can pull. That makes sense with 124 words. What is a reasonable plunge rate for basswood? Default is 12ipm. Cuts time from 9:44 to 6:21 if I go to 20ipm.

which Z axis do you have? HDZ/Z+ should be able to go prolly 2x faster

also a thing in carbide create: If you select many elements in one toolpath, the way it works is that it calculates the number of passes for the widest part of the whole toolpath, and ALL elements get that number of passes… small or large

If you have one wide part and lots of small ones… all the small ones get too many passes basically.

workaround is to split your toolpath in pieces, and do the bigger things separate from small text

1 Like

also there is an inefficiency in the gcode that carbide create generates for VCarve…
if you want to optimize that, you can try to use
https://fenrus75.github.io/FenrusCNCtools/ncopt/ncopt.html
with the “retract optimization”

Basically CC uses G1 speeds to get the Vbit straight up to your retract height, not G0 speeds… it’s not super far but every little bit adds up and with V carving of text you do this many many times

5 Likes

That looks like the ticket. I turned up the speed, but the major change was breaking up the artwork (which has thicker lines and takes more than one pass) and the text. Total time, including the outer contour, is now close to 2 hrs. More what I’d expect.

Haven’t tried the G0 modification as I’m not to post processing yet. Will do some tests to see what size font works.

Thanks,
Adam

1 Like