Hello Guest it is August 06, 2020, 06:48:41 AM

Author Topic: Homing and Home Offset  (Read 19597 times)

0 Members and 1 Guest are viewing this topic.

Homing and Home Offset
« on: February 01, 2014, 08:58:18 PM »
I've got my machine homing quite nicely now thanks to the members but I have 2 questions about the normal operating procedure and the Homing Offsets.

When I click on the REF ALL HOME after a reset my machine will home all 3 axis as well as run a home offset.

1) Should the normal procedure for the initial start up of the machine be to REF ALL HOME and if using the "Machine Coord's" click that button and zero all the axis? Does the Machine Coord's always need to be reset at start up?

2) My machine is set to inches and my Home Off. in the Motor / Soft Limits is set to 2.0 for x/y/a and -1.0 for z. After the REF ALL HOME I am assuming this is when I should see the offsets put into place however they are much smaller offsets than I have set, not sure what is not correctly setup, any ideas?

Thanks.

Adam,
« Last Edit: February 01, 2014, 09:04:04 PM by Adam_M »

Offline ger21

*
  • *
  •  6,282 6,282
    • View Profile
    • The CNC Woodworker
Re: Homing and Home Offset
« Reply #1 on: February 02, 2014, 12:55:40 AM »
1) The only way to rest machine coordinates is to home the machine. Clicking Ref All is all you need to do. You can';t zero machine coordinates any other way than homing.

2)The Offsets are in machine coordinates, so if you click the Machine Coordinates button after homing, you should see 2,2, and -1 in the DRO's
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Homing and Home Offset
« Reply #2 on: February 02, 2014, 07:15:21 AM »
1) The only way to rest machine coordinates is to home the machine. Clicking Ref All is all you need to do. You can';t zero machine coordinates any other way than homing.


So Machine homing has to take place at each start up of the machine or in the event something goes wrong in order for it to know where it physically is, correct? Essentially "REF ALL" sends the machine to the home switches where the axes can then be set to zero.


2)The Offsets are in machine coordinates, so if you click the Machine Coordinates button after homing, you should see 2,2, and -1 in the DRO's


This is exactly what it does from a visual perspective on the screen in the DRO's but the machine is not physically doing this, however the machine is not offset from the home switches 2", 2" , 2" and 1".


Adam,

Offline ger21

*
  • *
  •  6,282 6,282
    • View Profile
    • The CNC Woodworker
Re: Homing and Home Offset
« Reply #3 on: February 02, 2014, 08:44:00 AM »
Quote
So Machine homing has to take place at each start up of the machine or in the event something goes wrong in order for it to know where it physically is, correct?

Correct.

Quote
This is exactly what it does from a visual perspective on the screen in the DRO's but the machine is not physically doing this, however the machine is not offset from the home switches 2", 2" , 2" and 1".

This is also correct. When you set a "Home Offset" of "2", your telling Mach3 the switch location is 2, rather than 0. "Home Offset" doesn't add any movment to the homing, it just changes the location of the coordinate system.
If you want the machine to move 2" off the home switches, you'll need to add those commands to the Ref All script.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Homing and Home Offset
« Reply #4 on: February 02, 2014, 09:03:14 AM »
OK, very helpful.

One last question on the subject I hope..

Since a machine is physically limited in the x,y and z planes what is the purpose of setting a "Home Offset"?

For instance in my case I have them set for 2" and 1", if they physically don't set the machine's coordinates after a REF ALL then if I were to send a G code for a negative -3 or -2 in the Z axis then its going to hit the limit switches if I understand that correctly.

Quote
This is also correct. When you set a "Home Offset" of "2", your telling Mach3 the switch location is 2, rather than 0. "Home Offset" doesn't add any movment to the homing, it just changes the location of the coordinate system.
If you want the machine to move 2" off the home switches, you'll need to add those commands to the Ref All script.

Can you tell me where the Ref All script lives?

Thanks.

Adam,

Offline ger21

*
  • *
  •  6,282 6,282
    • View Profile
    • The CNC Woodworker
Re: Homing and Home Offset
« Reply #5 on: February 02, 2014, 09:25:10 AM »
OK, very helpful.

One last question on the subject I hope..

Since a machine is physically limited in the x,y and z planes what is the purpose of setting a "Home Offset"?



It allows you to define the Machine Coordinate system at a location other than where the home switches are physically located.

For instance, my router's X axis is 45", and my home switch is at the far right. I use a Home Offset of 45, so that X zero in machine coordinates is at the opposite end from the home switch.

Quote

For instance in my case I have them set for 2" and 1", if they physically don't set the machine's coordinates after a REF ALL then if I were to send a G code for a negative -3 or -2 in the Z axis then its going to hit the limit switches if I understand that correctly.


I think the term "physically" is a bit confusing here. The Machines coordinates are "set" to the Home Offset values.
Using the Z axis here is a bad example, as moving to Z-2 should be moving down, which should be away from the switch, as the Z home switch is typically at the top.

You need to consider where the switch is physically located as well.
If you set your X axis Home Offset to 2, and the home switch is at the positive end of travel, then you CAN move to -3. But if the switch is at the negative end of travel, then you can't go below 2, which is the switch location.

Quote

Can you tell me where the Ref All script lives?

Thanks.

Adam,

In Mach3, go to Operator >Edit Button Script, and click the Ref All button. THe script is in the button, saved in the screenset .set file.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Re: Homing and Home Offset
« Reply #6 on: February 02, 2014, 10:15:55 AM »
The controller,namely Mach, has an internal zero position and needs to allow one to define the machines zero position to it
since it does not know where the "physical" machines zero position is.

So the controller monitors axis movements from the moment it is turned on and after some movement to a USER defined position, and, upon the user zeroing all the axes, the controller can relate it's zero to the "physical" machines zero position. Picture two grids, one called software and the other called physical machine, side by side and then they are overlayed to one common grid with only one zero positioin to measure from, you have Machine Coordinate System. Machine zero should be chosen wisely for a number of reasons and may be at,on, within the user defined limits of travel. Hopefully this clarifies "physical"  for you.

I realy hate to muddy the waters, but remember this, it's the controlled point ie; the actual cutter location that is important and controlled, so all the
switch location stuff is just one consideration in defining the controlled point which is realy what the machine coordinates and programing is about.

You may read that a machines zero position is set by the manufacturer and can't be changed, but Mach needs to address
numerous machines and so it falls upon the user to define to the controller the info. Switches are used which automate the process of defining that info and thus they must be configured / setup.

So the switches provide for automating the process of homing the machine. The machine coordinate zero can't be changed unless you reconfigure the switches. Gcode commands provide for temporary and permanent of the controlled point.

The wording above is for general understanding and hope it helps and not confuses.

BTW,

By definition:

Machine Coordinate= Current Position + Work Offset + G92 Offset + Tool Offset
There is lot in the above simple equation.


FWIW,
RICH
Re: Homing and Home Offset
« Reply #7 on: February 02, 2014, 12:08:17 PM »
Thanks for the reply's, yes I think were now into theory/application and not machine specific answers.

Quote
For instance, my router's X axis is 45", and my home switch is at the far right. I use a Home Offset of 45, so that X zero in machine coordinates is at the opposite end from the home switch.

So, when you "REF ALL" on your machine your X moves all the way to the right to home, finds the home switch and then bumps off to the left, its now machine "Homed". The Home offset is set 45 to the left, so the grids that Rich suggested (good explanation by the way) are now different in the X by 45 mm/inches.

If you lay a piece of stock on your table to be milled without moving anything after "Homing", you have to find the edge of the material by jogging your X axis, correct?

When jogging your X axis to find the edge of the material is the Home Offset used for the machine to identify how far it has until it hits the "Home"  assuming you jog 25 (45-25 = 20)?

Offline ger21

*
  • *
  •  6,282 6,282
    • View Profile
    • The CNC Woodworker
Re: Homing and Home Offset
« Reply #8 on: February 02, 2014, 01:01:59 PM »
Quote
If you lay a piece of stock on your table to be milled without moving anything after "Homing", you have to find the edge of the material by jogging your X axis, correct?

Not the way I work, but for some people, yes.

I have a fence located at X zero that I place my parts against, so I never have to locate the edge. Well, almost never. My table also has a grid of threaded inserts that I sometimes use to bolt parts down. I have the table drawn as a template in my CAD program. SO I can create my toolpaths, place the part anywhere I want on the table, and it's ready to go.
My normal workflow is turn on the machine, home it, and it's ready to run parts. I don't zero to the edges.
When you zero to the edge of your parts, you're setting an offset. By default, Mach3 is in the G54 offset coordinate system. I keep my G54 X and Y offsets at zero, so I'm always actually working in Machine coordinates for the X and Y offsets.

Quote
When jogging your X axis to find the edge of the material is the Home Offset used for the machine to identify how far it has until it hits the "Home"  assuming you jog 25 (45-25 = 20)?

Home Offsets set the Machine Coordinate system on your machine to a position relative to your Home Switch position. As Rich mentioned, everything is then referenced from the Machine Coordinate system. That machine coordinate system never changes. If you start at 45 and jog to 20, then  you're at Machine Coordinate 20, and if you zero the axis there, then you are at G54 X zero. Basically, you set an offset of 20 for the X axis.


You might want to watch the video on Homing, Offsets and Limits.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Re: Homing and Home Offset
« Reply #9 on: February 02, 2014, 02:50:43 PM »
Link to the video:

https://www.youtube.com/watch?v=08qK4NfnXqA

---------------------------------------
BTW, I also work differenty than even Gerry. I don't use switches, but, most every thing i make on the mill is a one of a kind, no tool changer for it, etc. So i move to a logical spot where the CAM created a pre-compensated program code, zero / reference the machine, move a little away from the piece and let the chips fly.  Thus all coordinates systems are the same.

Not so with the lathe though. Still no home switches on it, do create a home position=machine zero position= tool change position, use work offsets, and do use soft limits to restrict axis movements sometimes.

-----------------------------------------------------------

What the above implies is that one can setup differently than another user. Yes there are standard ways of doing things.
So it's not theory, but rather an understanding how the controller works along with with what you or a program is telling the controller to do.

------------------------------------------------------------------------
Re-capping on what was said, the controller knows where Machine zero is and then the next step would be to define where the part is so the controller can relate to yet another "grid". Well call that grid, work coordinates and it's grid lies on top of
the machine coordinate grid, located where you told the controller it would be, and, the work coordinates are within
the limits.

RICH