Z height problems

[kjackswood]

I am having a slight problem with z height. I z down to the surface of the board to zero out before the program and then when running the program it cuts way too deep. I checked the depth of cut in v-carve and it was set to .10 but yet it drove alot deeper in the wood. I also have had problems with the toolpath preview in V Carve. no matter what I set the cut depth to in the tool path it still shows the cut going all the way down through the board.

Any advice on either problem would be appreciated

[jeb2cav]

What toolpath are you using? I suspect VCarve(?) I'll PM you with an email address.

[REG]

The depth is determined by the bit you select. There are ways to work-around the programed depth. Your dashboard on the depth is the toolpath. Select the area you want the bit to carve, select the bit then select calculate. Once calculation is finished close that toolpath window now you will have the detail information on the carve and the bit. At the bottom it will state the max depth of your carve. If this is too deep then double click the bit carve file in the toolpath and select a start depth of Z. Typically this is 0 but if you want to go deeper start with .010 if you want a shallower carve start with -.010 (minus). Another try is to change up bits say a 60 degree or a 40 degree.

Bobby

[jeb2cav]

Hi kjack and Bobby,

"The depth is determined by the bit you select" is not how I've found it to be or a good way for me to think about this. Don't get me wrong Bobby - that may work well for you and others. I discovered this before owning a CNC machine while trying my hand at the evaluation software. I tried what I thought was a simple sign, used the VCarve Toolpath, and cut through the wood.

What I learned about the VCarve Toolpath is that it cuts sides at the angle of the cutter you are using, to a depth until those two edges "meet at the bottom" (in a V). So, if you're using this toolpath to cut out lettering that has a big distance between them, there's a good chance you will "cut through" the material.

From the VCarve manual:

VCarve Manual Extract

I created a simple test with two sets of the same letters. The top letters are 4" tall, the bottom are 2" tall. The material is 0.25" deep. I used a V-Carve Toolpath, with a 90 degree 1.25" V-Bit, start depth of 0 and flat depth unchecked. Sure enough, this pass as set up cut through the material on the large letters.

Cut Through on Large Letters

To deny an opportunity to cut through the material, you have to set a Flat Depth in the V-Carve toolpath settings. Keep in mind though that you are going to also change the outcome - the cut may not (will not in this case) have a "V" bottom. The setting to change is highlighted in this graphic.

VCarve Toolpath Flat Depth.png

V-Carve Toolpath Flat Depth Setting

(11.55 KiB) Not downloaded yet

And now onto a separate post to complete the story (as this forum has a 3 picture per post maximum).

[jeb2cav]

Continued...

With the flat depth set to 0.2 in this case, the large letters look like this:

Large Letters Flat Dept 0.2

The small letters (1") weren't affected by the Flat Depth, so they still have a "V" in the bottom.

Small Letters Flat Depth Still with "V"

In this case, if you crank the Flat Depth to 0.05, the small letters also get a flat bottom.

Small Letters Small Flat Depth Flat Bottom

To be honest, this really confounded me when it happened. I tried resetting the tool cut depth, etc - before I took 2 minutes to read the manual on this toolpath, and had success. I felt pretty foolish at the time as I had spent probably more than an hour stroking buttons and previewing...

So, if you were using the V-Carve Toolpath, this should help. If you weren't using the V-Carve Toolpath and still have problems, let the forum know. Lots of knowledge and good ideas here.

Merry Christmas to all!

[kjackswood]

thanks again Joe and Bobby,

I think that is my problem is the flat cut and the other cut I need to be setting the bottom depth cut. The top cut should always be 0 if I understand it correctly.

Thanks guys

Merry Christmas to all.

[kjackswood]

Okay now I am confused,

I just upgraded to V Carve 6.0 yesterday, and just now tried to make a simple test program. and It appears the start depth and cut depths are different. The start depth at .10 instaed if 0 makes a shallower cut than setting the cut depth to the default of 1.0 which I set back to 0.0 to get a desirable cut in the preview.

[jeb2cav]

Hi Ken,

I still assume you are using a V-Carve toolpath. There is no real change in the panel choices between 5.5 and 6.0, but there may be some differences in default settings. In either case -

If you want the cut to be on the same plane as the top of your material (assuming you've set the origin of your project (default setting) on the top of the material), then yes, the "Start Depth" would be set to 0.0. If you had cut a pocket of 0.25", and wanted the lettering to be on the same plane as that, you would set the "Start Depth" to 0.25.

In this case, you'd have already cut a separate tool path using the Pocket toolpath. Then change bits, rezero the machine, and run the lettering toolpath (typically v-carve toolpath).

For a very basic project - a flat piece of wood with lettering, yes, the Start Depth would be 0.0. You'd only use the Flat Depth if you find that you're going to cut through the material (and you don't want to). If you have a wider angle v-bit - like 120 degree - you may find that it doesn't cut through the wood. Again, give the post above and the VCarve manual a quick look to see what is happening - in this case, the angle of the tool is going to drive how deep the actual final cut is (as determined by connecting the slope runs from each opposing vector).

[REG]

Hi kjack and Bobby,

"The depth is determined by the bit you select" is not how I've found it to be or a good way for me to think about this. Don't get me wrong Bobby - that may work well for you and others. I discovered this before owning a CNC machine while trying my hand at the evaluation software. I tried what I thought was a simple sign, used the VCarve Toolpath, and cut through the wood.

What I learned about the VCarve Toolpath is that it cuts sides at the angle of the cutter you are using, to a depth until those two edges "meet at the bottom" (in a V). So, if you're using this toolpath to cut out lettering that has a big distance between them, there's a good chance you will "cut through" the material.

I guess I should have been more specific, or at least the proper way to respond was to cover broader the size of the character can over-rule my response earlier. I was responding specifically to small characters. Carving a 1" tall character and selecting 90 degree V-bit, a 60 degree V-bit, and a 40 degree bit, each bit will give you different depths on the same charater. When the charater gets larger, the the narrower bits (40 degree and 60 degree) will have to make more passes and then the bottom depth comes into effect.
So, the proper response would be the size of the character, the type of bit and the depth settings can affect the carve depth.

Sorry for the confusion.

Bobby