Cutting a Taller Part

[tcgliderguy]

I've used Cut2D for several years, but have always been cutting fairly thin sheet stock. Now I have a project where I am cutting some fairly deep pockets into a 3 1/8" tall block of material. For some reason, if I set the Z zero point to the top of the block, the first move of the machine wants to raise the Z axis up 4 1/8"…. which crashes the Z axis into its vertical limit. If I se the Z zero point to the table top (bottom of the material) it still wants to raise up that 4 1/8" vertical move, and then come back down to cut.
I would really like to use my touch probe to set the zero at the top of the material….

Does anyone have a thought about where that initial 4 1/8" vertical move is coming from?

Thanks!

-Taylor

[JMD]

I've used Cut2D for several years, but have always been cutting fairly thin sheet stock. Now I have a project where I am cutting some fairly deep pockets into a 3 1/8" tall block of material. For some reason, if I set the Z zero point to the top of the block, the first move of the machine wants to raise the Z axis up 4 1/8"…. which crashes the Z axis into its vertical limit. If I se the Z zero point to the table top (bottom of the material) it still wants to raise up that 4 1/8" vertical move, and then come back down to cut.
I would really like to use my touch probe to set the zero at the top of the material….

Does anyone have a thought about where that initial 4 1/8" vertical move is coming from?

Thanks!

-Taylor

I have never used Cut 2D so I am not sure if this will be helpful or not. I V-Carvpro in the "Tool Paths Menu" under "Material Setup" there is a way to set the safe tool clearance in the Z Axis. Check to see what yours is set to. You may be able to lower it some to get away from your problem. Hope this helps.
John

[tcgliderguy]

Thanks for getting back to me….. I had the same thought, but in the Toolpaths Menu (for all four of the cutting operations involved) the "Safe Z" is set to 0.125 inches.

I finally prevailed, by eliminating line N170 from the code below. I have no idea why it was in there, but eliminating that line allowed me to make a test cut (in a block of wood, instead of aluminum) that came out perfectly….. Go figure?

Thanks for the help!

-Taylor

( Material Size)
( X= 14.000, Y= 3.500, Z= 3.125)
()
(Toolpaths used in this file:)
(REFERENCE HOLE)
(Main Pocket)
(Deep Pocket)
(Trigger Pocket)
(Tools used in this file: )
(1 = TC End Mill .25/.050/20)
N130G00G20G17G90G40G49G80
N140G70G91.1
N150T1M06
N160 (TC End Mill .25/.050/20)
N170G00G43Z4.1250H1
N180S12000M03
N190(Toolpath:- REFERENCE HOLE)
N200()
N210G94
N220X0.0000Y0.0000F20.0
N230G00X-0.0115Y0.0353Z3.2500
N240G1Z3.0750F30.0
N250G1X-0.0101Y0.0353F20.0

[Adrian]

It's the Home position of the Z that is doing this. Click on the material setup icon (the same place where you set the Safe Z) and look at the bottom right corner of the form. The Home Z is set there and that's the value used in the line you deleted.

[mezalick]

Make sure you recalculate the tool paths after changing the Z height.
Also, if you save this file after creating the new tool path, check the Z height on the next time you open up a new session ..
That new Z height may have been saved in the file.
Make adjustments as needed.
Michael

[tcgliderguy]

Thank You! This is the problem with being as time challenged as I am. I only get to work (Play?) with with my CNC stuff about every three months or so…

Somehow, on this project, I managed to skip over the Material Set-up tab……..

Thanks again for the assistance!

-Taylor

[Periproct]

Can I revive this thread? (And apologies in advance, its gone 01:30 and I've done a bit of damage to a bottle of wine).

I have my safe Z and home position Z set to 5mm. Every time I start to run G code in Mach3 (with the tool on the surface) the Z will go significantly more than 5mm and start to cut fresh air. I stop Mach3, jog the Z back down to the surface, rewind the G code, zero Z and the Z axis with go up 5mm and come back down and cut as normal. This is just a frustration as I have to set my tool to the surface twice but it would be nice to find a solution.
Regards, Nigel

[PaulRowntree]

What is the Z value on Mach3's readout before you ran the code, and what was it when you went back to the surface, prior to zero-ing it?

It isn't clear from your post: did you zero the Mach3 DRO's when the tool was first at the material top, before starting the program?

[Periproct]

I'm very careful to zero every axis once I have my tool on the surface. I have to confess I can't remember what the DRO shows on Mach3 but I'm sure it isn't correct as I have to zero Z again once I've got my tool back to the surface.
It is something as simple as I'm starting the G code with my tool at Z 0 but my material setup - home position is Z 5mm. (Rapid Z is 5mm as well). Although that doesn't explain why it'll work second time around.
I should really have waited until I'd make a note of how high my Z axis is actually going before I made my original post.

[Swdstmaker]

I had the same issue. The G43 code is tool length offset. Once set it stays active. The first run the z is compensated. Second re zero of the z resets it after the offset took place. I have been manually deleting the G43 command. I will try the material setup fix.
You can easily edit in mach3 by putting brackets around the line. ie (n170.......). It is treated as a comment then.

[Leo]

The G43 has a value associated with it -- it is the H.

The G43 looks for the H value that is set in the machine control.

If the H tool offset height IN the MACHINE - is set to ZERO - then there is NO offset and therefore the G43 will have NO effect in the CNC program and nothing needs to be done with it.

The problem the original poster was having was with the material setup.

[Mobius]

You can also remove the G43 command from your post processor completely by editing the post processor file and deleting the G43 line at the beginning.... it has saved me a pile of headaches.

Leo, where would a person find these tool offsets in mach 3? In the tool setup menu everything is zero, as it has been from day one with a fresh install of Mach 3 and Gerrys 2010 screenset, but I still suffer from the G43 command screwing things up. (Until I deleted it from the PP that is).

[Swdstmaker]

Thanks guys. Removing the G43 cures allot.
Zeroing the Mach3 Tool Table causes issues with other code not generated by Cut2D.
The G43 works perfectly if you have a CNC that always loads the tool at the same z position and the Mach 3 table matches your Cut2D table. Easier to remove it, or replace it with g49, which turns off tool length, just in case it got turned on somehow.

[sailor10]

N170 has a G43 code which uses the offset of the tool, in this case I think it was H4. I get rid of the G43 and the Hx from the line and it saves a ton of grief. Looking for a way to not have Cut2D make that line or somehow changing the tool database so it does not have a length for any of the tools.

[sailor10]

I think creating a g43 instruction should be an option that we can use or not use by choice. Something Vectric should think about.