60 degree vbit issues

[DC_CNC]

Hi All,

I've only had my Desktop Max for three weeks, and I'm having a great time working with it. I v-carved letters that are 1.1" high with a 60 degree vbit. Since the letters are so small, and since the vbit is so wide, it distorts the letters. For example, the inside of the letter "e" should still have stain in it, but the vbit carved it so much that the color is gone.

When I've cut the same font larger, it's fine, obviously.

Does anyone propose a solution? I figure I can try a 45 degree vbit it will be less, although the same depth.

Thanks.

[jTr]

Two choices: shallower depth of cut or pick a different bit with a more acute angle, like an 18 degree.

jeff

[Chuck Keysor]

Hello DC. I honestly couldn't figure out what problem you were describing, but after looking at your photo your issue became apparent. To at least start with a clear description of the problem, the little islands of wood that you want to remain within the loops of the script letters "e" and "l" are falling away/flaking off, taking their bits of attached surface paint/stain with them. That results in the visual defect you are encountering, and that is what you would like to prevent in the future.

The problem is not your bit, it is not the wood, it is not the stain. It is a combination of factors. Some types of wood and other materials may cut fine with your bit, and not have those little inner bits of the letter loops fall off. Other types of wood and materials could have been much worse. If for example, say you are cutting this text in MDF, some brands of MDF may hold these little details better than other brands............ And maybe with some other bit, but of the same carving angle, things may have turned out well. Maybe with the bit you used, but a different feed rate or RPM, or combination there of, things may have turned out OK.

This is where you have to learn what bits work with what materials, what feeds and speeds work, etc. This is mostly from your own experimentation. I used to have a stack of boards of different materials with test cutting designs on them, and some cut with different bits. Learning what works best come down to you experimenting and keeping track of what you discover works for you and your machine.

As a note, clear descriptions, and clear photos will be needed for you to try and get clear answers. Good luck and welcome to the forum, Chuck

[robtown]

Hello DC. I honestly couldn't figure out what problem you were describing, but after looking at your photo your issue became apparent. To at least start with a clear description of the problem, the little islands of wood that you want to remain within the loops of the script letters "e" and "l" are falling away/flaking off, taking their bits of attached surface paint/stain with them. That results in the visual defect you are encountering, and that is what you would like to prevent in the future.

The problem is not your bit, it is not the wood, it is not the stain. It is a combination of factors. Some types of wood and other materials may cut fine with your bit, and not have those little inner bits of the letter loops fall off. Other types of wood and materials could have been much worse. If for example, say you are cutting this text in MDF, some brands of MDF may hold these little details better than other brands............ And maybe with some other bit, but of the same carving angle, things may have turned out well. Maybe with the bit you used, but a different feed rate or RPM, or combination there of, things may have turned out OK.

This is where you have to learn what bits work with what materials, what feeds and speeds work, etc. This is mostly from your own experimentation. I used to have a stack of boards of different materials with test cutting designs on them, and some cut with different bits. Learning what works best come down to you experimenting and keeping track of what you discover works for you and your machine.

As a note, clear descriptions, and clear photos will be needed for you to try and get clear answers. Good luck and welcome to the forum, Chuck

Looks like you're cutting way too deep. Those e's shouldn't touch the l or the n. make sure you're table/spoilboard is good and flat, and that you get a good touch off when you set your z-zero...

Speaking of z-zero, do you z-zero from the table or the top of your material? In this case, I would zero from the top of the material, right there where you are cutting. At those letter sizes, even the tiniest variations in depth will yield less than desirable outcomes when v-carving.

[Red F]

It looks like the tool path is not set for a 60 degree bit, or your z is not zeroed correctly.

[scottp55]

What did the preview look like?
IF spoilboard is FLAT.
IF material is FLAT.
IF material is thickness specified and calipered correct.
IF the bit is a true 60 degrees.

It should look exactly like preview.
VCarve will NOT carve outside the lines! Only difference the angle of the bit does, is a 90* will carve shallower than a 30*.
It Always takes the angle of the bit into account....It doesn't matter if it's a .75" or .125" cutter....it will cut to the line and no further.

Basically the same machine as mine, and I routinely cut TT fonts down to .15" height in Franklin Gothic Demi in hardwoods, and can get SOME Scripts down to .16-.20"
The smaller you go, generally the steeper the bit, AND the less aggressively you can cut.
On the above heights, with an Onsrud 30* Engraving bit(not an upcut, so less tearout on TINY fonts) I'm all the way down to IPS .3(X,Y speed), .3(Z plunge speed), 18K(because it's a single flute) which Michael Tyler said he'd tried, so I did, and been using it for months without a single tearout on All kinds of hardwoods(including some soft Black Walnut sapwood a touch punky).
Bit stays cool to the touch...and it takes longer...but on one-of woods....I don't care:)

Helps when you get TINY to surface the wood ON your machine, and sand to finish grit(so you don't sand letter details off later), and sometimes for tearout, a coat or two finish will help(depending on finish).

MAY help to make a Font Board like I did the first month to find out what fonts actually carved like. Helped me a lot, AND helped explain to people about VCarving fonts, and why some are better than others.

Rambling again...You're still 4X larger on your font, than 60% of this stuff applies to.
I'm just avoiding going back in shop to fix a one-of, that somehow I spaced the pocket and made it .125" too big,AND make it look like I MEANT to do it!! :)

Desktop is a GREAT machine for Tiny stuff!! Congrats!
I stopped using the tool defaults almost immediately(kept them though)as they were a bit fast for my work, and just made my own category with feeds/speeds learned by testing.

[bobmoore]

show a snap shot of your vectors. I think you might be carving a single line font and choosing your cut depth incorrectly. your vectors will tell the story.
Bob

[chiloquinruss]

Play around with the 'Flat Depth (F)' setting when you select VCarve. Here's a really crude example. I didn't do a mini one but a large one to better show the effect of the change. 60 deg vbit used. BTW I have Aspire software. Russ

http://www.talkshopbot.com/forum/attachment.php?attachmentid=33062&stc=1 http://www.talkshopbot.com/forum/attachment.php?attachmentid=33063&stc=1 http://www.talkshopbot.com/forum/attachment.php?attachmentid=33064&stc=1

[cnc_works]

Given a proper setup (z zero set, proper bit chosen in tool settings), using vcarve it doesn't matter whether you use a 45deg, 60deg, or 90deg bit. None will go outside the vectors of the letter or whatever closed vector you are carving. The only difference in the carving is the depth of the point of the bit with the 45deg being deepest. So, it seems to me that your issue may be a z zero set too deep (a variation on this is if your material has moved up since setting z zero) or using a 90deg bit when you have the toolpath set for a 60deg bit. Also take a look at your vectors to see that they look normal for what you expect to see.

[EricSchimel]

That's actually not true if I'm understanding what you're saying...

When you do a toolpath for a V Carving, the angle of the bit determines the depth of cut, so if you take the exact same text and use a V Bit with a really wide angle, say 120 degrees, that bit isn't going to have to plunge very deep to "fill up" the space in between the vectors.

A much more "pointy" bit like a 30 degree is going to have to plunge much deeper to "fill up" the text:

33065

From the top, both the toolpaths look the same, but if you look at the side you'll see some very different depths:

33066

Same goes for V Carvings that have flat depths: Here we have too identical toolpaths with identical flat depths, one is a 120 degree bit and one is a 30:

33065

In addition to what others have suggested I'd make darn sure that your toolpath, and the actual V Bit you're using out of your tool database is correct.

Some bits have the angle called out from the centerline of the bit to one angled edge, Vectric likes the angle called out between the two cutting faces of the bit. Use an angle finder to be 100% sure you're not just punching in numbers on the box for the bit.

[cnc_works]

Don't know if you are replying to me, Eric, but it sure sounds as if we are both saying the same thing.

[EricSchimel]

I think we're saying the same thing now... :) I thought you might have been saying that any v carving toolpath can use any v bit.

I wasn't entirely sure so I figured I'd add a little bit if clarity.

[cnc_works]

Of course any vcarve toolpath can use any v bit. Though you may have to limit depth if the diameter of the v bit is smaller than the widest part of the vectors. The only difference in using different v bits is that the ones with the smallest angle will cut the deepest, and, of course, more pertinent is the need to fit the v bit to the design. In one inch letters I will almost automatically turn to a 60deg or perhaps even a 45deg v bit and in five inch or larger a 120deg bit. Choices are made both for depth of cut and also the way the light will hit the vcarving. At this point I don't know if I am clarifying or obfuscating.

[Chuck Keysor]

Hmm, there seems to have been a fair amount of conjecture as to the original poster's (DC CNC) problem. However, he never did come back with good pictures or clarifications that would help those who are trying to help him. Maybe someone offered him perfect advice???????? I hope so, Chuck

[woodshop]

Fine detail cutting is best at 0.045 - 0.075 (if you want to preserve the inside of small graphics).
Fonts are graphics and those E's and O's will be problematic at small sizes.
We cut with a 90 degree V cutter around here. (Too lazy to change bits for small details).
Soft wood can be weakened when you cut around it and then expect it to hold in place and not fall away.

0.045 - 0.075 max cut depth helps a lot!!!!!