Wondering if anyone has a solution to why my spindle will sometimes bury the bit straight down when I start a project. It has happened maybe six times or so in 165 jobs. I use the plate to probe XYZ. This last time that it happened I know for a fact that I probed all axis properly. Any help would greatly be appreciated. I don’t want to ruin a project because of it.
Edit: I also use top of work piece as my starting point.
Hey Nick, what kind of machine do you have (Elite?) Also do you use a tool setter?
Elite Journeyman and yes.
Have had the same problem about the same number of time.
Check to see if your job setup is for machine Zero or project surface Zero in the job size and position section.
Saw your edit.
Try the same file, then manually probe surface Z zero with a piece of paper. If you get the proper result the problem is the probe or probe settings
Thats my same setup and I had a similar issue a couple times until I realized what I was doing wrong.
Wrong Sequence:
Home machine
Change bit
Probe Z zero
Start my program which prompted me to change tools which I would just ignore and click cycle start since I already changed tools
Machine sets Z offset by tool setter
The problem being that the Z zero was set using the offset of the original tool length when I homed and not the tool I actually probed the Z with since I changed tools prior to the tool change prompt. Not sure if this is your issue but figured I would throw it out there. I realized that I needed to actually make a tool database which helps me double check what tool the machine thinks I homed with so I know where I am starting.
Do you home your machine after you set xyz? I believe that is recommended.
No I turn on my machine and then home it. I manually do XYZ with a plate.
I’ll give the sequence a try, thank you.
Try homing when turning on, and then home after setting xyz. If you are using Eazy-Z Tool setter.
You figured it out. ALL bit changes are based off of the first bit that is in there when you home and tool probe. After that it is just adding/subtracting the difference in bit length to get back to zero.
If you change a bit without commanding a tool change with M6, or change a bit and don’t touch off the probe your Z will be off. I did it too.
Now what I will do is manually command a tool change with M6 to whatever tool I will be starting the job with. When I load the job and the tool in use matches, it will just get started with the job instead of moving to the tool change position.
This also gives me a chance to send it back to Z0 just to confirm where that is before cutting starts, if it does the tool change at the beginning of the job it just goes right from the tool setter to cutting. Exactly how I broke the last bit…
I believe that this is related to your Z zero when probing and your Z zero in your program being different. The program zero is the top of the material for example, the machine is zero’d to the top of the spoil board. I’ve had this happen to me a few times as well, only to find out that when I created the program, I did not select the bottom of my part as the zero for my program. The other less likely issue is that the bit is sliding down, but this would normally occur during the machining when hogging out quite a bit more material and also using up spiral/compression bits in harder woods. I doubt that it’s the problem in your case. Let me know if this helps at all.
I too had this problem exactly. I homed the machine, then I used touch probe for XYZ with the tool needed and then started project. It went to the manual tool change position, I cycled start, it moved to Eazy Z touch probe to get another Z position. Then upon starting it plunged in and stopped messing up my project.
I reset and manually got Z went to work position and it worked fine.
I did these steps and so far it seems to work fine on my test runs.
1 - Power on
2 - Home Machine it will Auto Zero tool in spindle.
3 - Move to home and Zero Out XYZ
4 - Touch Probe XYZ for Project Location.
5 - Load File
6 - Rewind
7 - Cycle Start - Tool Change if required.
8 - Cycle Start - Auto Zero Initiated
9 - Program Runs to complete or until next tool change is required. Auto Zero should work from here on out.
I’m not following on step 4, would it not be either 3 or 4? I manually set xyz typically with out using the touch probe.
My 2 cents worth I had my spindle try to mill out my tool setter a few times after changing the tool manually and then homing, it went to the tool setter and did everything perfectly and stayed hovering over the tool setter. but when I pressed cycle start, it then tried to drill down through the tool setter. But if after homing I went to work origin and then pressed cycle start everything worked as it should I now always go to work origin after homing haven’t had a problem since.
Think your right. I do not think #3 is needed here as after homing XYZ machine coords are 0,0,0 already. It is the existing G54 coords (from last probe) that can get confusing as we think the display should show 0,0,0, but is showing some negative numbers because we are seeing an offset from the prior G54 origin and will likely be negative numbers if your sitting at machine Home location. But that is ok and expected. Your new work origin prob in #4 (or manual setup) will set your new G54 work origin and all should be good. Probably always good idea to press Go To Work Origin, just as a double-check and piece of mind, plus your not going to be over your tool setter at that point. If instead it jumps over to your tool setter location, something is amiss. I think I had that happen once, but I don’t remember what I did in order to duplicate it. I am sure I messed up somehow. Or maybe it was bug, not sure.