PDA

View Full Version : Artcam pro vbit carving



bbrad
10-01-2006, 06:57 PM
I am using artcam pro 8 and am trying to use the vbit carving. Seems simple but I am not getting a consistant depth of cut. I know that it is the material but I need to be able to adjust the depth of cut and I guess I just need as much info as anyone is willing to give. Can I make the changes as an off set wiht the shopbot? Or do the changes somehow in the artcam vbit section. Thanks, Bob

supertigre
10-01-2006, 10:00 PM
Bob;

The problem is not with the inconsistent depth of cut but your understanding of this feature.

In V-carving the depth of the bit is varied depending on the width of the line being carved. The wider the line, the deeper the bit needs to plunge into the material to make the line that wide. Have fun and play safe.

bbrad
10-01-2006, 10:49 PM
So if the cut is not deep enough in the artcam I can use the off set to make the tool cut deeperwith the shopbot.

paco
10-01-2006, 11:44 PM
"Seems simple but I am not getting a consistent depth of cut."

Elaborate please.

Why would you want to cut deeper than what it is suppose to?

The basic (for me) about V bit Carving is:

-to have the right angle tool bit as the one programed.
-V carving is surface work so one need to zero the Z at the top/surface of the material.
-One need as consistently flat material as possible.
-Weak hold down can create issue about inconsistent carving depth.

Now from your previous post, ArtCAM is ""WYSIWYG"" ; if it look good in AC, then it should be just as good on the material IF you do what you're supposed to...

Please, elaborate on the problem you're having.

Brady Watson
10-02-2006, 12:06 AM
Bob,
As Guy points out, depth is varied depending on the distance between the 2 vector boundaries that are being cut.

The other thing that affects carving depth is the angle of the bit. The higher numerical angle the shallower it cuts, and vice versa holds true with smaller angle bits. Try out different bits in Pro and take notice of the values it gives you on the v-carving toolpath tab when you select a tool and click on the centerline button. It will tell you the max depth & width that the selected tool will give you on the selected vectors. If you keep that tab open, you can keep selecting tools until you are happy with the depth value. The width value is practically of no use. If you find that the tool is going too deep for your material, then raise the numerical angle of the bit, which will result in a shallower cut. (IE- 90° cuts too deep for your material or takes too many passes to get to full depth ~ switch to a 120°)

Here's a rough 'recipe' that I use when doing v-carved signs and lettering. Use it as a rough gauge for your projects:

Text Height---- Recommended Bit Angle
< 1" ----------- 45° to 60°
1 to 2" -------- 60°
2 to 4" -------- 60° to 90°
4 to 6" -------- 90°
6 to 10" ------- 90° to 120°
Over 10" ------- 120° to higher°

Keep in mind that these are general guidlines that I personally use. They will function as a good basis for your own personal findings on your tool. Material thickness is a major factor in choosing bit angle as well as the diameter of the V-bit itself. If you are going to do a lot of v-carving in 1.5 or 2" HDU foam, then I recommend buying 1, 1.25. 1.75" diameter 60°, 90° and 120° bits from Onsrud, Gerber & Eagle America respectively. You can also buy insert type cutters from Her-Saf. A bit pricey, but they are worth it in the long run.

This should get you started...Hope it was of help to you & others.

-B

rick_woodward
10-02-2006, 09:18 AM
I think i know the issue Bob is refering to. I assume you have the zero plate and are using it to zero your bit. Then you run the toolpath but it dont look good in the thinner strokes of the letters. What i do is set my z depth maually. without the plate. carefully setting the bit right down on the wood. Click ZZ and you've reset your zero to the actual top of the wood. rerun your toolpath. This will deepen your cut and give you your thin lines like it should. Some fonts have very thin strokes on parts of the letters and dont cut deep enough to give a clean image. I have even set zero off the side of my piece by eye lower than the surface, mostly for a carving that i wanted a bit deeper. rick

bbrad
10-02-2006, 06:20 PM
Thanks for all the help. I was going to get the different degree cutters to get the best look.Also like the idea of setting z just below the suface as long as I manually lower the tool just a few thousands.