60 degree v-bit won't cut letters

[CCTDad]

I'm so frustrated. I'm trying to carve text with a new 60 degree Whiteside 1540 v-bit and I'm getting nothing beyond scratches in the surface of the stock, like it's a poor drag bit. I've attached the crv. I'm on a Shapeoko XXL running Carbide Motion, and if I create a text job in Carbide Create this bit cuts just fine. That leaves either the way that Carbide Motion digests the VCarve code, or I just have no idea what I'm doing. Probably the latter...

In the attached crv I set the flat depth to .5, .6, and .7 just to see what it would do. Barely a scratch in the surface of the wood--I can't even read it. Note that I only did this after having no luck at all with flat depth unchecked. I've calibrated using the Shapeoko touch probe as well as doing it the old fashioned way by bringing the bit down on the corner of the wood and it zeros perfectly. It knows where the surface of the stock is. Again, Carbide Create/Motion works just fine.

I had been thinking about buying Aspire. Now I'm just aggravated. Can anybody help? Do I just not understand the limitations of what I've got?

[scottp55]

Hoping somebody with your machine will chime in.
But, If you hover over all 3 toolpaths you'll see the depth on all 3 is .1133" deep...changing flat depth below that won't change a thing.
Depth is determined by space between the vectors and the angle of the bit in VCarving.
No problems I can see in program, but insufficiently caffeinated still:)

So machine setup in OS or Post Processor?
Somebody with same set up will probably help.
Don't get discouraged!
And welcome!
scott

[Bob Reda]

I ran them through simulation with no problem. Don't know why you have the flat depth checked. I got a depth of .08 which should work fine. I'm thinking your z may be off You also have to understand the material you are carving on. If it is wood the top more than likely is not perfectly flat. Now if you have about $20,000 in woodworking tools, you can make it so. In the meantime Is keep on fooling the z by dropping it a couple hundreds at a time and re zero it at that point go over what is faint. If need be drop it again and repeat. I do this quite often with wood to get the desired effect I'm looking for.

Bob

[Adrian]

You're misunderstanding the purpose of the flat depth setting. It's not controlling how deep the cut is other than to cut it off it exceeds that depth. As Scott says your toolpath is cutting to just over a 1/10th of an inch so it will never reach the flat depths you're specifying.

Given that it's running ok with your other software that eliminates a lot of possibilities. Are you using the correct post processor?

[sharkcutup]

An short answer to your problem -- Characters are not big enough to even be concerned with the Flat depth.

V-Carve is depth is usually determined by the size of the text character and its vector designed width. With the character set you have chosen the Characters would have to be approx. 8" tall before you are able to use the (F) Flat depth to control the depth of cut. In the image and file I have posted you can see that the v60 on the left cuts through the material because there is no depth set to control it.
The V60 on the right has been controlled using the (f) depth so that it does not go through the material.

v60 flat.crv

(1.77 MiB) Downloaded 89 times

As to the machine just scratching the surface What post processor are you saving the V-carve file with?

Hope this Helps!

Sharkcutup

[WNC_Ed]

If it is wood the top more than likely is not perfectly flat. Now if you have about $20,000 in woodworking tools, you can make it so.

I suppose the definition of "perfectly flat" would dictate what is required to get a surface flat. But if you have a CNC you can get it pretty darn close.
Certainly close enough to carve .5 inch deep letters.

[martin54]

As has been said already you are not really understanding the use of the flat depth option when using a Vcarve toolpath. If you hoover your curser over each of the 3 toolpaths you have created you will see that they all cut to exactly the same depth
If you want to carve deeper (using the vcarve toolpath) you would need to use a different font, make the letters deeper or use a bit with a different angle such as a 45 or 30 degree bit.

You are not cutting very deep to start with so if your stock is not perfectly flat & you set your z zero on a high bit of the material & your text is positioned on a lower bit of the material then it will not cut as deep as it should. Is your spoilboard perfectly flat & have you surfaced your material stock ?
I am not familiar with the program you have mentioned so don't know if that has the same sort of vcarve option or just an engraving option where you would set the depth of your engraving. You could try using the engraving option in the vcarve software to see if you get the same results as your other software

[wb9tpg]

I have the Shapeoko, use that exact bit, and I looked over your file. As pointed out by many the flat depth is never reached.

As to "scratching the surface", In order of likelyhood

• I'd say your machine doesn't have Z0 set correctly. Tell Carbide motion to move to 0 and see if the bit is on the surface. I'd guess it's not.
• Your bit is loose in the collet.
• The set screws on your Z are loose (not likely unless depth is changing)
• You Z axis belt is not tensioned correctly (not likely unless depth is changing)

When you say "scratching the surface" I take it you really mean barely cuts rather than a cut around 0.1" deepest.

[CCTDad]

Thanks everybody for your input.

First, WRT flat depth... let's just forget I mentioned it. I was just trying everything I could think of to get more, you know, depth, and this looked like a thing. Now I know that it's not. I was never trying to accomplish anything beyond experimenting with it anyway, so let's forget it.

I'm in a far-away time zone on a different schedule so I apologize for not getting back here sooner. I tried some things today with a bit of success, but I'd like to give some other stuff a shot tomorrow before I report back. In the meantime I didn't want anybody to think I wasn't appreciative for your help.

Thanks again,

-D

[edcasati]

If the letters are 'printing' too light, try increasing your "Start Depth" slightly. This will result in deeper and wider carves, but will not completely match the simulation.

These are the reasons that I have found for V Carve failing:
a) Wrong Z depth home. Boards are often curved, with the corners slightly higher than the center, or vice-versa. If you set your Z height at a high point, the bit might not even touch at the low point. The same can happen if your machine itself is not level to the material. Surfacing your material as a first step, with a 1 inch bit and a light in-place sanding is a for me standard step to get an even surface before running a V carve inclusive job.
b) Letters or designs are too thin. You need beefy images to Vcarve in wood. Thin designs just brush the surface, and the final sanding may make the image disappear.
c) Dull bit. If the bit is dull, on thin lines it will just push down but not cut the wood, since the Z depth may be minuscule.

If I want a really clear cut, I often use a 20 degree engraving bit and set a "flat depth" limit of 1mm or so. This will result in a deep cut with clean steep edges. You may need to run a 2mm flat clearance tool first since the tip of the bit is 0.01 mm. This takes paint very well.