Hello Guest it is December 12, 2019, 01:18:15 PM

Author Topic: Proper way to use work / tool offsets  (Read 300 times)

0 Members and 1 Guest are viewing this topic.

Proper way to use work / tool offsets
« on: March 18, 2019, 10:56:55 AM »
Hi all, this is more of a "teach me CNC" than a Mach 4 specific issue, but I was hoping to get your thoughts.

For the first time since I started this hobby, I have a machine with home/limit sensors. I used to just open Mach 3, zero the machine coordinate system at the work zero and cut away (all work offsets being zero). If the power went out and I machined off the corner I used to zero the part, then the part was scrap.

Now I turn on the machine, home to inductive proximity sensors, then home to the servo encoder marker pulse. This seems to be very repeatable - as it should be. My question is about how to properly use work offsets. After this homing sequence, I believe the machine starts in G53 and is located at 0,0,0. From there, I believe you can write gcode relative to a work zero defined in G54-G59. What it seems like I need to do is go into the MDI, enter G54, then edge find my part zero. When I zero this, does mach automatically and permanently save the work offset? Is there something I need to do in order to get it to be saved?

Now for tool offsets. I preset my tool lengths off the machine relative to the nose of the spindle. My code typically has a call like:
M06 T5
G43 H5
This loads the tool and height offset info for tool 5. Sometimes it seems like the first line runs and throws some weird number into the Z axis DRO, then when the second line runs, the correct tool position is reloaded into the DRO. I ran into an issue where this weird number triggered an error of being outside of soft limits even though the tool was perfectly well inside the limits.

What is the proper procedure to turn on the machine, home, locate the work zero, save the work offset, and handle tool length offsets?

Thanks!
Re: Proper way to use work / tool offsets
« Reply #1 on: March 18, 2019, 02:17:36 PM »
Hi,

Quote
I used to just open Mach 3, zero the machine coordinate system at the work zero and cut away (all work offsets being zero).

What was happening was that when you jogged to the start location and 'zeroed your machine coordinates' what you actually
did was 'home in place'. It is an option  (Mach3  AND Mach4) that when you <RefAllHome> or <RefAxis> to have the machines
current location be the new home position. It is a poor practice.

Now that you have proper home switches when you <RefAllHome> the machine will home and zero its machine coordinates.

Quote
I believe the machine starts in G53 and is located at 0,0,0

No, G53 is a non-modal Gcode that causes Mach to interpret the axis coordinate destinations on the line on which it occurs
as machine coordinates.

So you start a Mach4 session by starting the machine and hitting <RefAllHome>. Then jog to the start location, commonly
the corner of the material, and then 'zero the axes' per attached. Note that this zeros the work coordinates NOT the machine
coordinates. Mach does this by setting numbers in the current work offset (G54 by default) such that the current
machine coordinates MINUS the G54 offsets cause the DRO to be zero.

In the pic I have posted I homed the machine and then jogged 28mm in the X axis, 26mm in the Y axis and 22mm down
in the Z axis and then zeroed all three axes. The DROs all now read 0.0000  This means the work offsets (G54) are set to
28, 26 and -22. Thus the work offset is set without you having to do anything and you can now start machining.

Lets say you wish to run the same program again on the same piece of material (still in the vice) you can use the button
<GoTOWorkZero> and the machine will traverse to the corner of the material. You might consider then that the G54 offsets
are the machine coordinate location of the corner of the material. The DROs should all read 0.0000 and you can now run
your Gcode again.

Lets say you want to finish the Mach session without completing the part. When you shut Mach down the work offsets
are flushed to the registers which are stored in the .ini file. Lets say you come back the next day. Start Mach and the work
offsets will be restored to what they were at the end of your last session.Home (<RefAllHome>) as normal and then
<GoToWorkZero> and the machine will traverse to the corner of the material which is still in the vice. You don't
have to touch off again.

Note that Mach3 and Mach4 behave the same in this regard. I fact ALL CNC machines operate this way. It is for this reason
that I argue that good home switches are ESSENTIAL to operating Mach. In your case you have added index homing to the
mix but the essential idea remains the same. The work offsets (G54, G55, G56...etc) are in effect the machine coordinate
locations of various points of interest, the corner of the material in the vice for instance.

Quote
Sometimes it seems like the first line runs and throws some weird number into the Z axis DRO,

When m6 runs the DRO will change to the current work coordinate location of the Z axis. The number represents the difference
between the actual and current machine coordinate and the current work offset but with NO tool offset. When the second
line runs the tool offset is set per the attached and the DRO recalculated to include the G54 offsets AND the tool offsets.

Craig

My wife left with my best friend...
     and I miss him!
Re: Proper way to use work / tool offsets
« Reply #2 on: March 18, 2019, 03:42:00 PM »
Craig, this was just what I was looking for. Thank you.  I will have to play around with the offsets and try resuming a program after powering down.
Re: Proper way to use work / tool offsets
« Reply #3 on: March 18, 2019, 05:10:20 PM »
Hi,
I had used Mach3 for a year or more without home switches......and all this stuff was very confusing to me. I had
a few crashes too.

Then I got around to fitting home switches and in short order the fog cleared.....and I've had only one crash in the 4-1/2 years
since, operator error.

May I suggest using the Offsets page and expand the Fixture Table and observe the effect of entering data directly
into the Fixture Table and using the Machine Coords button to flick back and forth between machine coords and work coords.
Note you can pin the Fixture Table to the top, and keep it in view while you experiment.

Craig
My wife left with my best friend...
     and I miss him!
Re: Proper way to use work / tool offsets
« Reply #4 on: March 19, 2019, 08:44:34 AM »
Home switches make everything nice!!!
I agree with Craig, dig in and experiment, it's the best way to learn.

mcardoso,
Have you seen the Mach Support YouTube Channel?
https://www.youtube.com/channel/UCcZ847PqPXOUrksLYct-gaA/videos

Tool Offsets
https://www.youtube.com/watch?v=tywAByswH2Q

Work Offsets
https://www.youtube.com/watch?v=0aRifYB70Mc&t=95s
Chad Byrd
Re: Proper way to use work / tool offsets
« Reply #5 on: March 19, 2019, 09:05:50 AM »
Craig and Cbyrdtopper,

Thanks much for the info! I watched all those videos last night and they really helped! I think at this point I just need some spindle time with the fixture table open to see what is going on. Does Mach 4 support the extended work offsets beyond G59?
Re: Proper way to use work / tool offsets
« Reply #6 on: March 19, 2019, 10:09:49 AM »
Hi,

Quote
Does Mach 4 support the extended work offsets beyond G59?

Yes. Open the Fixture Table and scroll down.

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