[jcrouch]

I can't find anyone that has had the problem I am having. I don't know if it is in Mach3 or the 2010 screen set. here is the problem.

The feed rate doesn't change on the machine when the file runs and I think I am doing the code correctly. This is an example of the code I have been using. I want this to make a keyhole to hang a plaque I made. I think the speed is going break the keyhole tool, so I haven't tried it, Just air cuts.

I can set on the 2010 screen set feed rate override to different settings and the when the file runs there is a change, but all F commands are the same speed. I can speed it up and down. but it doesn't work when the file runs. I have been working on this for 2 days and just can't find the answers. Can anyone think of what I can do. I have attached an XML file (I HOPE) with the setup for my machine (I think)
Thanks for any help you can come up with.
Jim
P.S I have changed the feeds to all kinds of different numbers. This is where I stopped.

N001 G0G43
N002 S1200M08
N003 G94F0.05
N010 G90Z-.1083
N015 G91X-1F0.05
N020 G91X1F0.05
N025 G91Z1F100
N030 (G00)
N035 M09
N040 M09
N45 M30


This is the specs on my unit
3X3 fine line automation FLA 250 It's not a 200 or a 300 it is about 32" X 32" almost
Gecko G540 4 axis stepper motor driver
48V 12.5A switching power supply — the current needed for a 4 motor system
4 High-torque Nema 23 380 oz-in stepper motors. Have not used the last motor yet.
HITACHI M12 VC Router
Mach3
Vcave Pro I could do it with a gadget but I would like to place the bit over the place I want the keyhole and not have to go to vcarve pro each time I do another hole.

[jcrouch]

or Does anyone know of a good g code tutorial?

[ger21]

The G0 in your first line is causing all the subsequent moves to move at rapid rate, so the feedrates aren't being used. You need to use G1 for the feedrates to work.

I made some other changes.
Removed G43, as you didn't have the complete command in there, which would be G43 Hxx.
Added G20 (inches) and G40 (disable cutter comp just in case)
Increased spindle speed to 12000 from 1200 rpm.
Replaced M8 with M3. M8 is coolant, M3 starts spindle.
Replaced M9 (coolant off) with M5 (spindle off).
Removed G0, and added G1 to first move.
G0 and G1 are modal, and remain in effect until changed.
Removed some of you F0.5, as feedrate is also Modal and remains in effect until changed.

This code should run fine.
However, my guess ids that a feedrate of 0.05 will burn up your keyhole bit, and may even start a fire. I think a feedrate of 20-30 ipm would be more appropriate for plunging, and I'd probably cut the slot a little faster, maybe 50ipm?

Also, be very careful mixing incremental and absolute modes, as you can get in a lot of trouble that way.


N001 G94 G40 G20
N002 S12000 M03
N010 G90 G1 Z-.1083 F0.5
N015 G91 X-1
N020 G91 X1
N025 G91 Z1 F100
N040 M05
N45 M30

Also, feel free to email me directly if you have questions on the screenset.

[ger21]

or Does anyone know of a good g code tutorial?

Take a look through the manual. (Or click the G in the toolbar of the 2010 Screenset, which I think lists the g-codes word for word from the manual).

What I'd do is create some basic parts in V-Carve Pro, export the g-code, and study it to see what's going on.

[jcrouch]

Gerry,
Thank you
On line 'N002 S12000 M03'
I have to use M08 or M802 (a macro) to start my router. That is how I have it hooked up.
Say I could have another switch if I change that. I'll have to look that up next.
Thanks again
Jim

[ger21]

I have to use M08 or M802 (a macro) to start my router. That is how I have it hooked up.

Go to Ports and Pins, Spindle tab, and you'll see you have spindle CW set to use Output 3. Change it to Output 2.
Then check the box to disable coolant, and you can then use M3 to start and M5 to stop the spindle. You don't need to change anything else for your spindle to function correctly.

You might also want to go to General Config, and uncheck "Boxed DRO's and Graphics", and "Auto Screen Enlarge", then close and restart mach3. The 2010 Screenset will then be displayed as it was intended.

[jcrouch]

Gerry
That was going to be my next question. Do you do mind reading on the side? this is wonderful every thing is working. Now I have to change my vcarve pro pre-possesser back to the way it came. You have been a great help. It's like finding a Genny in a bottle (BTW) how many more wishes can I have.
Thanks again
Jim

[shujaa]

Dear friend,

you are a very nice person. i am using your screen set. and i am very happy.

thanks a lot.

Live long and Prosper.