Group - On most of my cuts the Z axis does not quite cut through the material. It is about 2 thousandths short of cutting all the way through.
Although I set the cutting depth two thousandths deeper than the material thickness, my cuts are still not complete all the way through the material.
I am running a CNC Router Parts router with Fuchs limit switches.
Before each cut, I use a touch probe that is calibrated to the correct height.
The machine is returned to home before each cut.
The material is that the router is failing to cut through is a consistent thickness
The table has been planed flat
V-carve pro alerts me that that I am going to be cutting through the material
I measure the material thickness with digital dial calipers and set the material thickness as indicated
Are you setting your Z-zero to the spoilbard (i.e., bottom of your material)? That would normally assure a complete cut-through if all else you mentioned is true (spoilboard surfaced flat, touchplate thickness correct, etc.).
I am setting the Z-axis at 0 by referencing the top of the material with the touch probe. Then in the Vectric Pro software, I input the material thickness. As a point of curiosity, the last cut I even instructed the Vectric program to cut 2 thousand of an inch deeper than the material.
I suspected that the 1" thick CNC router parts touch plate was not actually 1" thick, but dial calipers measured it to be exactly to be 1". With this in mind, I suspected that the script used for the touch plate Z-axis zeroing was incorrect, but it too is set to reference a touch plate at exactly 1".
To diagnose the problem, I will do some test cuts with everything set like my last cut that left the 1-2 thousandths material but zero the Z-axis the old fashion way with paper and see if the problem persists.
Do you have any additional thoughts on tests that would be helpful to diagnose this situation?
Lots of things can cause this.
As the tool gets dull, it may push the wood down a bit.
The spoilboard can compress under the plywood, or actually get thinner with humidity changes.
The machine could flex a few thousandths.
As the spoilboard wears, you'll need to cut deeper.
On our $150,000 machine at work, I start with a new bit, and clean spoilboard, cutting about .003" through. I gradually increase the depth as the spoilboard gets cut and the bit starts to wear, sometimes cutting as much as .01" through.
If you're only talking 1 or 2 thou, then maybe your Z axis calibration is slightly off.
Attach a dial indicator to the Z axis and confirm that it is actually moving the distance that it's being told to.
A couple of years ago we changed over to cutting everything setting z-zero to the table. When doing cutouts this eliminates issues with variability in material thickness. When doing pockets and carvings we do have to carefully mic the material, but it hasn't been an issue. Another advantage is that it has completely prevented issues we used to have when we would change from z0 at bottom to z0 at top and then forget to change the machine back before the next run that was supposed to have z0 at bottom, resulting in gouges and broken bits (and once, a fire). Gary Campbell told us to pick one and stick with it, and that's been good advice.
Steve Godding
Not all who wander (or wonder) are lost
Did you try a test cut by setting your file to Z-zero bottom of material and using your touchplate to set Z-zero to the spoilbard/machine bed?
Shops that are regularly cutting sheet goods typically *never* set Z-zero to the top of the material. Sheet goods can vary in thickness and/or don’t lay perfectly flat. Zeroing from the spoilboard assures a full cut-through if either of those conditions exist.
Did you try a test cut by setting your file to Z-zero bottom of material and using your touchplate to set Z-zero to the spoilbard/machine bed?
Shops that are regularly cutting sheet goods typically *never* set Z-zero to the top of the material. Sheet goods can vary in thickness and/or don’t lay perfectly flat. Zeroing from the spoilboard assures a full cut-through if either of those conditions exist.
+1.
These days I only cut 8x4 sheets and several a day at that. I always zero to the spoilboard top and set the toolpaths to overcut by 0.1mm. No issues at all that way with nice clean bottom edges using a DC bit.
I'm glad this discussion is being held. I usually cut solid wood and don't have an issue if the cut isn't completely through the material. Most of my projects allow me to use a pattern bit to clean things up and especially since I use tabs. I'm getting ready to do a couple of projects in plywood and want to make a complete through cut. This will give me an opportunity to do the work differently by using the spoilboard top.
The only thing I picked up on was that you used a dial calipers to measure your touch off block.
Not besmirching dial calipers, but that sort of error is within their tolerance depending on who is using them. It also depends on the quality of the dial calipers. I use them all the time, but when I am doing actual precision machining work I get out the micrometers.
Frankly, if this is a consistent problem I would just tell the software that the block is 1.002 thick and see how that works out.
"If you see a good fight, get in it." Dr. Vernon Johns
If you're using a compression bit for sheet goods the advice we've always gotten is to go through the material into the spoilboard to get a clean bottom cut. We use .009". Don't really care if we "spoil the spoilboard". It's there to be spoiled. Just flatten it periodically. Taking .010" off each time it's flattened, a spoilboard lasts a reasonable amount of time.
Steve Godding
Not all who wander (or wonder) are lost
