Hello Guest it is December 12, 2019, 02:39:49 PM

Author Topic: Probe not stopping "Z" axis  (Read 3139 times)

0 Members and 1 Guest are viewing this topic.

Re: Probe not stopping "Z" axis
« Reply #10 on: October 21, 2017, 10:01:16 AM »
Hi,

Just got a little bit lost with this G-Code I generated using from an Eagle design using PCB-Gcode, When running the code as in attachment,Commands "R0.1000 cause an error "R Less thanY in XZ Plane" this is in line 47.

G82 X-0.8000 Y2.4000  Z-0.0320 F20    R0.1000  P1.000000

Also what is the P1.00000  ???,   "P    Serves as parameter address for various G and M codes    

    With G04, defines dwell time value.
    Also serves as a parameter in some canned cycles, representing dwell times or other variables.
    Also used in the calling and termination of subprograms. (With M98, it specifies which subprogram to call; with M99, it specifies which block number of the main program to return to.)"

 Can I delete both these command as R seems to relate to an arc.

Also stops on the "M03" command "To fast for pulley using Max" but carries on think that may related to spindle set at "S20000" which is not running on this test and is prob way faster than my spindle, so just need to edit as required..

Regards John
Re: Probe not stopping "Z" axis
« Reply #11 on: October 21, 2017, 01:56:02 PM »
Hi John,
G82 is a canned drill cycle with dwell.
The P is the dwell time when the drill get to the bottom.
R is the retract height. You are expecting that the drill tip starts out at 0.1 inch, that is above the board, it drill down at 20 in/min until 0.032 inch below the top
of the board, dwell for 1 second and then retract at rapid  rate to Z-0.1 ie 0.1 inch above the board.

All of these values are set when you set-up PCB-Gcode. What thickness is your board?, I would guess it is 32 thou or 0.8mm. Your drill, if everything is perfect,
is going to get to the bottom surface of the board but not penetrate it. Is that what you want? I use 1.5mm PCB and I have the drill go to Z=-1.8mm so
it reliably penetrates the board and I'm quite OK with the drill digging into the spoil board below. Dwell only need be 0.25 sec or so.

The only real error in the code you've posted is that your machine is in XZ plane mode? You want to be in XY plane mode. Try putting a G17 to select XY plane
mode right at the very top of the Gcode job, I'm surprised that its not already active with all the preparatory codes.

If you think that you can do CNC jobs without being able to read and understand basic Gcode... you are wrong. It is a required skill that you be able to understand
little chunks of code like this example and be able to understand what your machine will do when it encounters it. On the Program Run page there are two buttons
to provide concise notes as to the meaning of G and M codes. The CNC bible is:
Quote
CNC Programming Handbook by Peter Smid
its a dry read but very good. No doubt there are other texts and probably plenty on the net, find them and
read them, we are not born being able to read Gcode, it something we have to learn. If the value of a hobby is what you have to learn in pursuit of that hobby
the CNC rates very highly...you have to learn untold things to be any good at it.

Craig
My wife left with my best friend...
     and I miss him!
Re: Probe not stopping "Z" axis
« Reply #12 on: October 21, 2017, 04:04:58 PM »
Hi Craig,

I realize that I will have to learn the G-Code it'll take a bit the old grey matter is not the same as when I was younger.

I have re-done the PCB Gcode from Eagle for the Timer PCB without any changes so you can see if there is any errors, all I will have to do is put the G17 at the beginning.

My CNC settings for "Z" are on the DRO 0.0000 at the top and goes down by about 2.75 inches so -2.7500, thats just before limit to limit switches.

I have a G-Code listing from CNC Cookbook so will use it to go through and try and understand what is happening.

Regards John
Re: Probe not stopping "Z" axis
« Reply #13 on: October 21, 2017, 04:33:16 PM »
Hi John,
I notice you are using a Z drill depth of 0.062 inch, ie 1/16 inch. If you are using 1/16 inch circuit board its not enuf, if you are using 1/32 PCB then
the drill will penetrate which is good. Are you happy that the drill will mark the material underneath?

Next issue is this confusion about the Z axis co-ordinates. It is very common to define the very top of Z axis travel as MACHINE co-ord 0. Your
Z axis can go 2.75 inches lower so your machine co-ord at that point would be -2.75.

When you are machining a PCB you'll be in WORK co-ords. Notice the Gcode you posted shows a Z of 0.1 inch when above the board, but that's higher than
the very top! So the Gcode you have posted is written in work co-ords. It expects the top surface of the board to be Z=0 Then Z=0.1 means a tenth of an inch
above the PCB and Z=0.005 as 5 thou below the surface, probably the cut depth of a router bit if you are mechanically etching the board.

So the procedure is to set the PCB blank in its jig and manually jog the spindle down until the tool just touches the surface of the blank and then hit <Zero Z>.
Now set the code to run, any positive Z means above the board and safe and any negative number means the tool/drill is engaged with the workpiece.

Craig
My wife left with my best friend...
     and I miss him!
Re: Probe not stopping "Z" axis
« Reply #14 on: October 21, 2017, 04:41:13 PM »
Hi John,
no disrespect for the Gcode publication you got but if you wanted to know about the Quran, for instance, would you read it in a popular magazine or would you
get a genuine copy? In like manner Peter Smid's book is the authoritative source.

Craig
My wife left with my best friend...
     and I miss him!
Re: Probe not stopping "Z" axis
« Reply #15 on: October 21, 2017, 06:09:36 PM »
Hi John,
just noticed a typo which could throw you out...

I wrote Z=0.005...it should be Z=-0.005   The negative sign is critical to understand...negative Z below the surface, positive Z above the surface.

Craig
My wife left with my best friend...
     and I miss him!
Re: Probe not stopping "Z" axis
« Reply #16 on: October 22, 2017, 10:33:23 AM »
Hi Craig

Okay done a dry run on that G-Code and changed a few parameters, and it works fine Ive not run spindle motor yet will try that on Monday, like you said added the G17 then changed R and P settings as they were to long and it goes through cycle brilliant.

Got to do mods to Y gantry as its to much movement the 8mm bars just have to much bend so getting 12mm supported and fix the Y gantry to the base so X axis moves and prob change the Y axis bars to 12mm bars.

Also found that need to add Probe script to set the Z high off a work piece, got that off a YouTube Guru.

The book is a very good idea but at £56 on Amazon will have to be a present, I think I have a fair understanding of this G-Code will learn more as I use more.

Regards John
Re: Probe not stopping "Z" axis
« Reply #17 on: October 22, 2017, 12:06:54 PM »
Hi John,
I got a download of the book, not as convenient as printed but OK.

Craig
My wife left with my best friend...
     and I miss him!
Re: Probe not stopping "Z" axis
« Reply #18 on: October 23, 2017, 06:51:34 AM »
Hi Craig,

I would be interested in the download link.

Also been looking for program to allow me to use a Web cam mounted in place of the Spindle motor so I can program co-ordinates from a PCB Negative Photo of board ( the old method before Gerber came along) and create G-Code, have you ever come across anything, Ive been searching but cant find anything.

Thanks again for Help

Regards John
Re: Probe not stopping "Z" axis
« Reply #19 on: October 23, 2017, 07:03:46 AM »
Hi John,
check out the Video Probing board of the forum.

I use Eagle software to produce PCB artwork then there is a User Language Program (PCB-Gcode) which converts the artwork into Gcode.
I personally have not seen any program that can take a visual image of a circuit board and produce Gcode. It sounds more like something
people doing artistic engraving might know something about.

Ill try and find a link for the book. I see my copy is 140Mb so it won't attach to an email comfortably.

Craig
My wife left with my best friend...
     and I miss him!