Yes … Z zero at spoil board on Vcarve Pro.
I understand to do a X,Y,Z zero before starting the job. This also applies to BitSetter.
Does a X,Y,Z zero, or Z zero need to be done before or after Bitsetter?
I might be missing the point of your question, but the BitSetter is all automated. Carbide Motion will run the BitSetter routine after “Initialization” homing. It will then run the BitSetter routine when you start the job when each tool change is called.
You just set your zeros after the “Initialization”.
Then start job.
1 Like
Ok got it … now to figure out why my Z plunged.
Can you share the Gcode?
Change the .extension to .gcode
The Heart Box Lid Top worked.
The Heart Box Lid Bottom … the Z plunged.
The difference from the Top Lid and Bottom Lid, Top Lid referenced at top of material, Bottom Lid referenced at Machine Bed.
Heart Box Lid Top.pdf (560.7 KB) Heart Box Lid Bottom.pdf (2.2 MB)
I wanted to clarify something for everyone with the V-Carve posts and the BitSetter.
There is a redundant BitSetter sequence at the start. I think Carbide3D is in a tough spot, trying to anticipate all the ways we can jack up their new accessory.
Personally, I don’t use the M6 command for the first tool. In Carbide Motion, this saves me the redundant BitSetter routine.
Issues with that: When I first published the posts (without the redundant BitSetting), several reported the issue with Motion where it says you’re using one less tool than you are and claims that the first tool used is actually the second in your gcode. I get it…if you read that stuff, or, even worse, rely on that information, it’s a bit confusing. I think CM could get around this by looking for the active tool (T) word instead of the M6 for that list. @robgrz @Luke
Another issue would be those that might like to probe zeros with something other than the first tool they’re using.
I’m not sure what the answer is or the direction I should take the Post Processors (no M6 for first tool or keep the rendundant M6?).
If there are two versions(easy enough to do)…what do I call them?
Any input is welcome.
2 Likes
How thick is your material?
Stock Z axis?
Yes, redundant … That’s what I encountered and it is confusing.
1.77" thick is my stock thickness.
Do you have an inch of clearance (Z-travel) above it?
It just is cutting too deep on the outside profile?
I zeroed my Z using the first tool (1), 1/8 endmill. Then a tool change after the 1/8 bit job was completed to tool (2), 1/4 endmill. Then the Z plunged to a depth of 0.4 with a gcode plunge depth set for 0.2. Then it plunged deeper thus changing/increasing the bit length as can be seen by a black sharpie mark on the bit shank that I used as a reference.
I have 3/8" of travel from the tip of the bit to the top of the stock.
The outside profile is set to cut a lip of about 0.2" depth, with 3 passes. Last pass I set for a 0.02" final cut.
Here’s a pic of the gcode order.
I am not sure if for some odd reason the gcode order changed that it is cutting the outside profile, .
I don’t see anything in the code. You may be losing position on the slotting.
If it happens again, stop the job and see what happens when you jog to Z0 (careful…if you’re losing Z height you might crash).
If you let it go, does it cut into the wasteboard? (This would indicate a loss of position)
I’ll have to pass this one off to the late night shift.
Thanks Neil … I did not let it go … I shut it down … I’m just bummed because it’s 3 pieces of Maple glued together. The only piece of $$$ wood I have.
I need to think this one over. Redo the gcode, and keep it simple. No final pass.
1 Like
I think I found my problem based on the above quote and what you last posted, Z losing position.
My Vcarve Pro Z1 is set for a clearance of 0.7" above the stock. My remaing clearance is 3/8". The Z lost position … based on this I would assume.
If this is the cause then another lesson learned in the world of CNCing.
1 Like
That’s why I asked. 
I think I misread this:
I thought I saw a 2.77 in your gcode.
If you crashed the Z on the retract, that explains it.
1.77 is my stock thickness … I think I crashed the Z on retract based on my Z1 clearance setting of 0.7".
The stock is 1.77 + 0.7 = 2.4".
The total measured travel from tip of bit to full retract is 2.125".
This explains my crash that caused my Z to lose position. Thanks for helping me find this root cause of my issue.
Glad its not the Bitsetter and zeroing from the machine bed vice the top of the stock.
1 Like
Reran the job … ALL is good.
Thanks Neil for ALL your help … Problem solved …
3 Likes
Is there a reason for having CM to initialize a tool change (Bitsetter sequence) prior to running a job?
It would make sense for a tool change (Bitsetter sequence) to start once you decide to run a job and not before.
Does this have anything to do with what Neil is mentioning in the above quote?
Is the redundancy caused by Vcarve Pro? I have not tested a similar gcode created by CC to see if it is an isolated redundancy issue with Vcarve Pro and not CC.