z axis jogging?

Post anything you want to discuss with others about the software.

z axis jogging?

Postby badgersurfer » Tue Jan 31, 2017 10:33 am

I am making items in hardwood that are 50mm x 35mm x 6mm. I generally run the blanks which are on average 200mm long across a planer and then a thicknesser to get my thickness smooth and accurate. The problem with this is that it is time consuming. I found that if I just put the rough blanks in my Stepcraft 420 with a 3mm end mill I can mill off a relatively clean surface with a 50% overlap in seconds. This saves me a lot of time and effort. I then finish with sanding.
I have created a template in Vcarve Pro as follows. Pocket toolpath cutting at a depth of 0.025 mm across the workpiece surface.
At the moment I am rewinding the toolpath file and resetting the tool height to take another .025 cut. What I want to achieve is to be able to jog down 0.025 after each run until the surface or thickness is where I want.
I am obviously not doing this correctly. I assume that if I type in the z axis line .025mm it will move down to the correct amount and then run the toolpath again.
Is this the easiest procedure or is there a button I can customise to jog down .025 just with one click?
badgersurfer
 
Posts: 10
Joined: Tue Nov 22, 2016 10:32 am

Re: z axis jogging?

Postby Vmax549 » Tue Jan 31, 2017 5:02 pm

AN easy way to do that is to Make teh Z step depth a #var such as #100. Use it as for example

G1 Z#100 F5 ( Lowers Z to the value of #100)

Before you run each pass, From teh MDI line, assign a value to #100 such as

#100 = -.025

Then you run teh program and teh Z will step down to -.025.

IF you need to run it again adjust the value of #100 to a lower depth.

(;-) TP
Vmax549
 
Posts: 1104
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: z axis jogging?

Postby badgersurfer » Tue Jan 31, 2017 9:29 pm

Vmax549 wrote:AN easy way to do that is to Make teh Z step depth a #var such as #100. Use it as for example

G1 Z#100 F5 ( Lowers Z to the value of #100)

Before you run each pass, From teh MDI line, assign a value to #100 such as

#100 = -.025

Then you run teh program and teh Z will step down to -.025.

IF you need to run it again adjust the value of #100 to a lower depth.

(;-) TP

Thanks, I will have to try and get my head around what you are saying here as I am new to uccnc... As a matter of interest can I utilise e.g. G55 (in it is on the interface to do this.
I notice that by default the program always assigns the G54 button. This seems to take on the Z=0 settings. So I thought that if I assign the G55 button to z -0.025 and then clicked it before I rerun the toolpaths it would do what I wanted, but I don't think it does as when I run the toolpath again it always seems to start at the 0 coords assigned in the vcarve toolpath.
I tried it but when I ran the toolpath in Demo mode it always seems to start at zero and not -.025
badgersurfer
 
Posts: 10
Joined: Tue Nov 22, 2016 10:32 am

Re: z axis jogging?

Postby Vmax549 » Tue Jan 31, 2017 10:14 pm

it is possible to do it that way BUT you only have 6 work offsets to work with where as you need 9.

ANother similar method would be to this way. You do not need to set anything via MDI the code will step down each time you run it. But you do need to assure that #100 = 0 before you make teh first run.

MDI #100 = 0

Then you start running teh code. At teh end of each run if you need to go further simply restart teh program again(CycleStart)

G90
#100 = [#100 -.25]
G0 X0 Y0 Z.3
G1 Z#100 F5
G1 X5 F20
Y5
X0
Y0
M30

OR This way where you do NOT have to do anything with a MDI Just keep running teh program until you get to where you want.

G90
G0 X0 Y0 Z.3
G91
G1 Z-.25 F5
G90
G1 X5 F20
Y5
X0
Y0
M30

There ARE many way to do this. You could also use SUB programming (;-) TP
Vmax549
 
Posts: 1104
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: z axis jogging?

Postby cncdrive » Tue Jan 31, 2017 10:23 pm

I assume that your g-code program does not contain any Z movement and is in absolute motion mode G90, if so then there is a simple way to implement what you want is to add a few lines at the end of your code:

G91 (switch to incremental motion mode)
G1 Z-0.025 (move the Z with -0.025 units increment)
G90 (switch back to absolute motion mode)

The code will not work good if your g-code program contains any Z movements, because then the Z will move back to that height when you rerun your g-code.
cncdrive
Site Admin
 
Posts: 2113
Joined: Tue Aug 12, 2014 11:17 pm

Re: z axis jogging?

Postby spumco » Wed Feb 01, 2017 5:51 am

Is there some reason why you can't just set the step jog value to .025mm (or whatever you want) in the jog panel and then jog down one step before re-running the surfacing program?

If your program doesn't have any Z-moves this should be the 'one button' solution you want.

If it does have Z- commands, then edit the program to end at Z0 and rewind. Then jog one step and re-zero the Z-DRO. Re-run program as many times as you need. If you forget to re-zero after you jog down a step you'll just cut air for one cycle - no crashes.

Maybe I'm overlooking something here.

-S
spumco
 
Posts: 174
Joined: Mon Oct 03, 2016 10:10 pm


Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 3 guests