Page 1 of 1

Spindle wont go up to clear surface at beginning of job

Posted: Tue Apr 19, 2016 2:30 am
by jfboyd
Any idea why my spindle wont go up at the beginning of a job to clear the stock surface? It just go straight from zero to beginning of the job. If surface is not 100% levelled, it will scratch it.

I just changed my board for the new one to fix the disconnect issue. I thought it would fix this too, but it's still doing it. Im creating my Gcode with Create.

Thanks for your help!

Re: Spindle wont go up to clear surface at beginning of job

Posted: Tue Apr 19, 2016 3:37 am
by WillAdams
Carbide Create seems to use:

Code: Select all

G1Z-0.883F293.4
for a safety margin.

Not much unless your machine and stock are perfect.

One thing to check is Z-axis belt tension.

You could edit the code by hand.

I'd suggest filing a feature request for configurable safety margin.

Re: Spindle wont go up to clear surface at beginning of job

Posted: Tue Apr 19, 2016 3:40 am
by jfboyd
Thank you! I will do that !

Belt tensions seems to be good.

Re: Spindle wont go up to clear surface at beginning of job

Posted: Tue Apr 19, 2016 3:43 am
by WillAdams
It also starts off lifting up:

Code: Select all

G0X0.000Y0.000Z12.000

Re: Spindle wont go up to clear surface at beginning of job

Posted: Tue Apr 19, 2016 4:33 am
by DRobs86
I dont use Create, but I did experince this in Fusion 360. I usually edit the g code to lift to whatever clearance I desire. Another option which I also use is to just start above stock zero at my desird safe height. It will traverse in the xy plane and then move down to your first cutting depth as long as you are running absolute coordinates.

Re: Spindle wont go up to clear surface at beginning of job

Posted: Wed Apr 20, 2016 2:30 am
by jalapano
I did experince this in Fusion 360. I usually edit the g code to lift to whatever clearance I desire
Can you explain what steps you do edit the gcode to life the it to a safe level. It'd be really helpful, I've hit the problem too.

Re: Spindle wont go up to clear surface at beginning of job

Posted: Wed Apr 20, 2016 5:27 pm
by DRobs86
Open G code file in text editor. You may have to rename with a .txt extension to open with notepad (other options too ,but i will keep it simple).

The header of the file will include commands such as:
G90 G94
G21
G17
M3...etc
Then your first xy traverse:
G0 X143.2 Y23.9. (Just as an example, could be any x and y value

Before that first xy traverse, enter a new line and type:
G0 Z6 (6 is just an example, you can use any value you want for a safe height)

Save the file.

There are a couple other ways to handle this, but thats an easy one. Be very mindful though that fusion likes to throw a G54 in the header (still trying to stop that myself, I am sure I need to just look into it). If you are in another work coordinate system (G55, etc) and expecting to run in that, then you are in for trouble. I also delete the G54 command from the header so that I stay in the work coordinate system I selected before running the file.

Re: Spindle wont go up to clear surface at beginning of job

Posted: Fri Apr 29, 2016 3:11 am
by jalapano
Thanks! (sorry for being late, been super busy)

I'll have some time to try it out this weekend.