Occasionally, not always, my Z axis will drop at the very beginning of my tool path and ruin the surface of my work piece. I have CC V7 pro. Attached is a pic of the g code when it starts. I can see the Z is set to drop on line 8. I have tried deleting this line and it still happens.
Does anyone have any suggestions?
What design software? If Carbide Create, post a file here where you have seen the problem.
If you run the same file twice, does the problem happen both times?
Post the matching .c2d file?
Step-by-step notes on how you are securing your stock and setting zero relative to it and managing all tool changes?
Post a photo showing an attempt at cutting still in place on the machine with the machine at the origin or a specified offset from that position?
Which machine? Which Z-axis?
I ran the same file twice and it happened both times.
Carbide Create V7.
The machine is a Onefinity.
I am securing the stock with drywall screw and ensuring that it isnât lifting in the middle with a level on top of it. I set zero with a oiece of paper .01 above the stock. This problem started occurring when i upgraded to V7 of CC.
I have been doing the paper trick for years on multiple machines.
I have tried several places on my table and it occurs anywhere.
Neon_Avery_NAMEONLY.nc (2.8 KB)
Are you sure that movement isnât supposed to be in G53 (Machine) coordinate space?
Post the .c2d file?
Before the XY move?
Thatâs not in your gcode. If itâs dropping before an xy move, thereâs something else going on.
That Z move is weird because itâs rapid. Post that c2d file and one of these guys will look at it.
Deleted due to inaccuracy.
I donât how to make it start higher than Z0. This is how i have always used it. It doesnât always happen.
My retract height is set to .5" which always works fine.
I have tried to set my Z0 and move it up prior to start but it will drop Z and then move XY and still cause the issue. Should i edit the g code manually for each file to raise it at the beginning? Is there something within CC that can do this?
I may be incorrect in my first reply. I am not sure if the rapid is in XYZ as one move. If two, first XY then Z, my response was incorrect ( I have deleted it).
If it is dropping in Z before any rapids, you have an Infinity machine problem. As Neil stated, there is no move in Z before XY in your code.
You should not have to edit Gcode.
Your file setup is:
when the post-processor is set to âBasic G-codeâ and metric
and G-code is output using build 767:
The first few lines are:
G90
G21
(Toolpath:...)
(Toolpath:...)
M05
M0 ;T10
M03S15000
G0X47.653Y96.623
Z-2.750
G1Z-4.588F203.2
X48.295Y96.443F2159.0
So it rapids to 2.75mm below the stock surface before beginning a movement at the plunge rate.
Ii may be that this is a bug, and if so will put it in as that, but I forgot to check the Start Depth of the toolpath â naturally if that is set to 2.75mm, then the program is doing what it is asked.
That makes sense. I think itâs a bug as well because i never had this issue until i got V7 of CC. I used it for over 2 years with the same machine before this ever happened and i always set up the same way.
If lines 8 and 9 are interpreted as two moves, wouldnât the bit have been directly above the start point prior to the rapid in Z to -2.75? If so, the Z rapid should not cause the cut across the surface that James is seeing.
The rapid in Z to -2.75, looks like a normal move to a âsafeâ position above the start of the contour cut (-4.20mm in the C2d). No?
The start depth is set to 3mm, so this move while rather aggressive should still be âsafeâ.
I would expect it to rapid to the retract height (+12.7mm), then plunge to first cutting depth (-3mm - 1.587 = -4.587)
The two tool paths have different starts . One is 4.2 with a max of 4.21 and the other is 3 with a max of 21. I think the prior is the path in question based on the photos.
Bozo is correct. The path with 4.2 and 4.21 is the one that messed up.
If the two look similar with respect to movements, and one is okay, one not, this should help troubleshoot. I have to go to a real job nowâŠCheers.
So you have a start depth of 4.2, and the tool is rapiding to -3.95. That should still be safe, since youâre telling the software that you have already machined down to -4.2.
If youâre wanting it to make a pass at 4.20, and another pass at 4.21, then you should set
DOC: 4.2
Start Depth: 0.0
Max Depth: 4.21
Thank you Tod1d, ill try that.