I just recently made a few plaques that had odd depths in some of the carves. I’m running a 1/8 Endmill with a V30 for the advanced carve design, but on some of the letters the endmill goes down every so slightly shallower than the V bit does so the center pocket area can be raised above. I haven’t seen this problem before in my carves. I’m manually doing the Z-zero and then the machine does the bit setter for the tool change. Any thoughts why I’d get different depths in the same pocket? Only thing that makes sense to me is the bit setter is slightly off? I’ve been doing manual zero since I’ve found it to be more accurate (at least for the X/Y).
You could check the bit setter on a test piece to verify the zero is the same (or within a reasonable tolerance).
The other thing I’ve seen in my limited time with my CNC is the wood will sometimes warp as a relief is cut into it. Granted when I have seen this I am cutting fairly deep into the material so I doubt a “normal” v-carve would cause this but possible. Is the issue consistent all the way around the carve?
1 Like
Happy birthday Chris!
I don’t think it’s wood warping/stressing. The cut depth is only .02 on a 3/4" piece so it’s not enough for that. The issue is definitely consistent through several letters. The initial endmill is definitely not as deep as the V carve.
Thanks!
Ah yes, .02 is not going to introduce anything in that kind of stock thickness. I would check the bitsetter to verify it is repeating. When I installed mine, I created a file with two tools in it. I just copied my 1/4" endmill and gave it a new number.
Then I machined a relief .200 into a piece of Azek (what I had on hand at the time). Next, I set the second tool to machine at a start depth of .190 and depth per pass of .005 down to .210. When I got the “tool change” I just moved the same tool in the collet and continued. Then I noted when the tool actually touched the material. It shouldn’t cut anything until the third pass… .190 first, .195 second and .200 third. Mine just BARELY touched at .2. I ran it a few times to verify results.
Oh, I almost forgot, after machining the first relief I checked the depth with a depth mic to be sure I had a .2 deep relief.
I’m guessing you have been using the bitsetter previously, so we are checking for any “Drift” in its performance now.
Here’s some photos so it might make more sense. I’ve been using it for awhile now, but I like your function testing. I’ll give that a try after dinner. I measure the difference which came out to be .01. This isn’t a crazy difference, but it’s obviously enough to pick up visually. I just circled the most obvious spots.
Could this be mechanical? Is there any vertical play, either in the spindle / router, the Z Carriage, or slop on the X Carriage?
My Z leadscrew right now has about 1/2mm vertical slop.
1 Like
Wow, thanks for the pics. That is not what I was envisioning. I was thinking the flat was flat but at a different depth consistently. I’d have a look at the machine Z axis as suggested above. I was trying to see if it looked like a speed/feed issue but it doesn’t look like it to me. Stupid question but any chance the bit is dull? Again, no pattern as far as grain and mill pattern goes that I can detect but something odd for sure.
Good luck!
So when you set up your first bit (end mill correct?) are you using a bit Zero device or the paper method for your Z height?
I ran the test we talked about 3 times. The accuracy was well within tolerance that it wasn’t detectible without running a fingernail over it and even then it was barely noticeable. Therefore, I doubt this is a mechanical issue as we’ve been thinking. There’s got to be something about the V bit that’s throwing the depth in the software off I would think? I’m using an Amana 1/4" shank V30 bit so it’s a quality one, but I have no clue at this point.
Correct, EM to start. Then swap to V30. I have done both methods with the same result.
How did you enter this? Using what feeds and speeds?
So I’ve been having the same or similar situation where my V-bit being just slightly deeper then my pocketing end mill. I don’t have Bit Zero or a Bit Setter for tool changing. Been using depth collars until just recently and still a sheet of paper to find Z zero on my stock. I always have to remember to turn on the vacuum to my spoil board because the foam gaskets I use allow the stock to sink about .6 mm.
I’m just thinking out loud here, if you use a sheet of paper to set Z zero with your first end mill bit installed, then use a Bit Setter with a the V-bit at tool change, perhaps? there’s depth difference that’s created by the Bit Setter in relation to the Z zero height. Just enough to see and actually feel with your finger nail.
And this will sound really off the wall but I finally solved my depth difference by fabricating two different depth gauges for the bit change (I have a Makita). First one I use to chuck the end mill, sheet of paper Z zero, then the one I use to chuck the V-it is just around .4mm shorter. I know it sounds odd but the height is now the same.
Christopher can you post your file please.
Anthony
So that makes sense, but that’s sorta compensating for an issue we should be able to fix. Weird for sure.
backer v30.c2d (284 KB)
Here’s the file
The 1/8 EM is 8 plunge/20 ips/ 0.05 DOC
The v30 is 15/75/0.05
Christopher
Part of your problem is the diameter of your bit and the actual width of you letters.Look at the W and you will see the cleared circles in the larger areas that is the area that the 1/8 bit can cut and this cut deeper or the deepest as in your pictures. If you change to a smaller bit 1/16 and view the simulation again you will see more area removed. This is also in several other letters and the design above.
look at the test file I made the bit change in the first tool path only and see the change in the cuts and simulation.
Anthony
Chris test file 1-16 bit.c2d (272 KB)
I added a 1/8 inch box near the W and this represents the size of the 1/8 bit and when you place this over your letters you can see it is larger than some areas of theletters and the bit will not cut anything smaller that the box.
1 Like
So I understand that the larger bit can only cut so much of the smaller letters, but changing the bit to a smaller size only allow more clearing… not depth changes right? We’re just talking about being more efficient with a smaller EM for clearing the flat areas, but that wouldn’t have any impact on the V30 going deeper, unless I’m not seeing something? In theory, if nothing else changed… I’d just being seeing a “bigger” circle since the 1/16th bit can cover more ground.
Wish I had more time today as I am thinking exactly Anthony is. However, I would think the advanced vcarve would be smart enough to use the v-bit to clear the sections the endmill can’t get into. Having said that I have very little CC advanced vcarve to compare. I’ve been using vcarve pro and it does clear anything the end mill doesn’t using the v-bit (or a smaller endmill if you prefer/need).
Also, there is no issue using the paper to zero and the then the bit setter. I’ve done this tons of times. All the bitsetter is doing is comparing the tool length and creating an offset to apply to the tool path z axis information. So if your zero is correct with tool #1 then it will be fine for tool #2, 3 and so on.
Chris
The smaller bit will clear more of the lettering and should let the V bit do its job of clearing the walls of the letter.
Chris M
For both Chris C&M
That’s exactly what Advance V carve does with the proper tooling and bits. If you clear out all the bottoms with the correct diameter tools and have the vbit set up correctly it will leave a smooth bottom and sharp corners on the side walls.
In this case you were using the Vbit to clear out all the bottom with a step over of .008.
Chris C see if you can get a really good close up picture of the letter W and show the bottom and the walls clearly and post it.
I think once you change the tool to the 1/16 bit and do a test cut you should see a very good cut then.
Anthony