Home Search and Offsets Question

# Thread: Home Search and Offsets Question

1. ## Home Search and Offsets Question

Hi Everyone,
Kind of a newbie question here.

I am setting my my 4' by 8' router table controlled by a F8025M. I've just finished setting up all the parameters associated with the "Machine Reference Search."

When I finish a machine home, the "Machine Reference Zero" point turns out to be at X=-6.365, Y=-0.134, and Z=5.75 with respect to the actual origin (corner of) of my 4'x8' table. Here's a rough diagram where "M" is the machine reference Zero point and "o" is the origin (corner of the table):

........|......................................| ^
........|......................................| |
........|......................................| Y
........|......................................| |
M......|o_______________________| v
.........<----------- X ------------>

What is the best way to set up my parameters and post processor with offsets, etc. to account for the difference between these two points?

My first thought is to set parameters P119=-6.365, P219= -0.134, and P319=5.75 (basically the machine assigns these values to X, Y & Z respectively during the machine home). Next, a G00 X0 Y0 Z0 is done to move the spindle to the corner of the table. Then I can use a G59 X0 Y0 Z0 for my offsets.

Would this be the correct way to do this?
Is there a bettery way?

If I do this, will G90 moves still be referenced to the M point as the 0,0,0 point or will the G90 moves be referenced to the corner of the table?

Thanks for any help or suggestions.
R/Todd
Last edited by TAProwler; 08-19-2011 at 11:43 PM.

2. Hot Rolled
Join Date
Apr 2009
Location
California
Posts
519
Post Thanks / Like
Likes (Given)
3
14
That's beyond my knowledge with the Fagor. G59 I guess gives you the option of programming another offset zero point, and move all of your offsets to another zero point.

There's so much the control will do that I have yet to learn.

3. Diamond
Join Date
Dec 2007
Location
Southeastern US
Posts
6,225
Post Thanks / Like
Likes (Given)
728
2589
On any control the typical procedure is as you describe, set it to actual position relative to reference origin to get your desired 0,0,0 physical point. (Your P parameters listed above.)

4. ## OK, Thanks

Hey Tony,
Thanks for confirming. That's what I thought.
I will give it a shove in that direction.

Anyone have any insight on what that will do to the reference point for my soft limits and absolute moves (G90's)?? Will those operations then be referenced to the corner of the table? That seems logical.

If nothing else, I'll just set it up - then try it and see.

Thanks.
R/Todd

5. Hot Rolled
Join Date
Jun 2008
Location
Roanoke, VA
Posts
615
Post Thanks / Like
Likes (Given)
181
208
Our lasers and plasma both home off of the sheet, though the origin is the corner. If you tell it to go home and it sits over the edge of the sheet itt you be hard to get the waste sheet out and a new one in. You may just have to try some things and see what happens.

6. Diamond
Join Date
Dec 2007
Location
Southeastern US
Posts
6,225
Post Thanks / Like
Likes (Given)
728
2589
It will regard the 0,0,0 as origin and all G90 moves will be referenced to that 0,0,0 position.

7. Cast Iron
Join Date
Apr 2007
Location
Haverhill, MA
Posts
335
Post Thanks / Like
Likes (Given)
84
113
Originally Posted by TAProwler
Anyone have any insight on what that will do to the reference point for my soft limits and absolute moves (G90's)?? Will those operations then be referenced to the corner of the table? That seems logical.
Forgive me if this is way below your current level, but you mentioned that it was a newbie question, and it seems to me that something is being missed (either by you or by me).

g54 through g59 are work offsets that can be set to any position. They basically say "the origin of the part is, for example, 5 inches in each direction from the reference position. These can be changed to any location you want. The machine reference position is, according to the manual, an offset from the machine home position. A g53 would (usually temporarily) force the machine to make moves off the reference position.

So...

G54 G90 G0 X0 Y0 would make the machine move the the zero point you set for G54. This works for G55 through G59 as well. These are modal, and will be remembered until you change it. Many controls support additional work offsets by appending a digit, for example G541, G542, etc...

G53 G90 G0 X0 Y0 would make the machine move to the machine reference point. G53 is usually one-shot, so it must be included on each line.

G90 is an "absolute" move with reference to the current work offset (g54-g59), NOT compared to the machine reference position. The current work offset can be set to the reference position via G53.

Soft limits are global and reference the machine reference position. Work offsets do not effect soft limits.

Again, it seems to me like that's what you're asking, but I could just be totally missing the point. If that's the case I'll shut up and go do something else. I just thought it was odd that you jumped right to G59.

EDIT: unless you're asking about using G59 as an additive offset (when parameter 619 is set to 1). I've never used that...

Also, the manual for that control sucks.

8. Diamond
Join Date
Dec 2007
Location
Southeastern US
Posts
6,225
Post Thanks / Like
Likes (Given)
728
2589
I understood the question to mean "will my Gxx offsets in G90 mode reference the corner of the table where I want my X0,Y0,Z0 to be physically located if I set these parameters as I've stated". - And the answer to that question is yes.

If the OP meant something else, please clarify.

9. Cast Iron
Join Date
Apr 2007
Location
Haverhill, MA
Posts
335
Post Thanks / Like
Likes (Given)
84
113
I was confused by this:

If I do this, will G90 moves still be referenced to the M point as the 0,0,0 point or will the G90 moves be referenced to the corner of the table?
combined with this

Then I can use a G59 X0 Y0 Z0 for my offsets.

I only posted after reading the manual for that control, which does a really bad job at explaining work offsets (in fact, it doesn't explain them). Figured I would throw it out there just in case.

Yeah, everything references the 0,0,0 you set in the *19 parameters. The position it finds as "home" no longer exists in its own right after those are set.

10. ## Great Discussion - That is My Question!

Sniper & Tony,

Thank you very much for your insight(s).

Sniper - your offsets discussion helped to clarify a lot. I don't have lot of experience using offsets yet and I'm not completely certain how they relate to the physical position(s) of/on the machine.

Tony - You have really cleared up my question of how to define where I want my origin (0,0,0) point to be .vs. where the machine reference point is determined by a machine home.

You have both addressed what I'm short of knowledge on. This is the first machine that I have set up and I probably understand the physical / mechanical aspects of this better than the software/G code aspects - particulary with respect to offsets.

This is the way that I understand everything so far:

1. When I perform a "Home Reference" the machine homes each axis by moving the axis until it's associated microswitch closes. Then it slowly moves the axis in the opposite direction until it finds the next (closest) marker pulse from the servo encoder.

2. When this is complete on all three axes - the machine now "knows" exactly where it is. However, this is not where I want the X=0, Y=0, and Z=0 point to be (It's off of the router vacuum table).

3. In order to get the machine to have the (0,0,0) point on the table, the controller has parameters that can be set to "assign" a position (on the DRO) to each axis at the completion of the home reference described in step 1. above. By doing this - whenever my G code now has a G00 X0 Y0 Z0 it will move the spindle to the origin point on my table.

4. It now seems logical to me that (with the machine set up this way) the soft limits will be referenced to "my" origin (the X=0, Y=0, and Z=0 point). It also seems logical that all G90 moves will be referenced to this same point.

Question A: Do I have this all right so far?

Now, my confusion with the G59 comes from this:
If, instead of doing the setup above, I left the machine reference point ALSO be the X=0, Y=0, and Z=0 point; then I could use G59 set so that using this offset will put me on the corner of the table. The offest would have to be G59 X6.365 Y0.134 Z-5.75 (I presume).

My controller also has a parameter setting that will allow me to set it up so that any G54-G59 offset will give me the offset defined by G54-G59 PLUS the G59 offset.

This all would affect how I have to set up my post processor. I would have to define the G59 offset correctly in each post to ensure the router was on the table. It makes more sense to me, to set up the machine the way that I descirbed in 1-4 above.

Question B: Is the setup described in 1-4 above the industry accepted standard practice here?

I hope I have not confused the issue more. If the answer to Question A above is yes, then I think I'm starting to get this all sorted out. If the answer to question B is yes, then it's a slam dunk.

Thanks for your help.
R/Todd

11. Originally Posted by sniper1rfa
I only posted after reading the manual for that control, which does a really bad job at explaining work offsets (in fact, it doesn't explain them). Figured I would throw it out there just in case.

Yeah, everything references the 0,0,0 you set in the *19 parameters. The position it finds as "home" no longer exists in its own right after those are set.

Sniper, I just re-read your last post and saw that you have answered my questions. Thank you for your "really bad" comment - I thought it was just me. Maybe I'm not as "thick" as I thought.

CASE CLOSED!
Thanks a lot for your help.
R/Todd

12. Cast Iron
Join Date
Apr 2007
Location
Haverhill, MA
Posts
335
Post Thanks / Like
Likes (Given)
84
113
Originally Posted by TAProwler
Sniper - your offsets discussion helped to clarify a lot. I don't have lot of experience using offsets yet and I'm not completely certain how they relate to the physical position(s) of/on the machine.
Those will be something you set in the control while running it. They do not need to be pre-set. If you have five parts, for example, you will set the origin of each part by edge-finding or whatever, and put those origins in the offsets table. You'll be changing them constantly. You use work offsets so you can use the coordinates straight from your print, rather than adjusting all your numbers. It also allows you to put the part anywhere you want on the table without changing your program.

This is the way that I understand everything so far:

1. When I perform a "Home Reference" the machine homes each axis by moving the axis until it's associated microswitch closes. Then it slowly moves the axis in the opposite direction until it finds the next (closest) marker pulse from the servo encoder.
Yes.

2. When this is complete on all three axes - the machine now "knows" exactly where it is. However, this is not where I want the X=0, Y=0, and Z=0 point to be (It's off of the router vacuum table).
Yup.

3. In order to get the machine to have the (0,0,0) point on the table, the controller has parameters that can be set to "assign" a position (on the DRO) to each axis at the completion of the home reference described in step 1. above.
yup.

By doing this - whenever my G code now has a G00 X0 Y0 Z0 it will move the spindle to the origin point on my table.
Not necessarily. As described above, the values for X and Y will reference the zero point you set in your work offsets (G54-G59). Those need to appear in the code before any moves you want to make with reference to them. They are "modal", which means they stay active until you call something else. You will generally use these any time you're cutting parts.

If you want your coordinates to reference the corner of the table, which you set as 0,0,0 in the parameters, you need to call a G53. G53 effectively cancels your current work offset temporarily (for the line it's on). The line after your G53 line will typically revert back to the last work offset you were using. That's called a one-shot command. You usually use G53 to move the table to a position where you can work on it - for example bringing a vice forward after the program is finished so you can change parts.

Now, my confusion with the G59 comes from this:
If, instead of doing the setup above, I left the machine reference point ALSO be the X=0, Y=0, and Z=0 point; then I could use G59 set so that using this offset will put me on the corner of the table. The offest would have to be G59 X6.365 Y0.134 Z-5.75 (I presume).
The line "G59 X0 Y0 Z0" does not *set* the current location. That would physically move to 0,0,0 under the G59 work offset in whatever mode the machine is in (either feed, G01, or rapid, G00).

My controller also has a parameter setting that will allow me to set it up so that any G54-G59 offset will give me the offset defined by G54-G59 PLUS the G59 offset.
Yes, i noticed that. I recommend setting that parameter (619) to "0" and using G59 as a normal work offset. If you have reason to change it later you can, but I think for now it would be too many layers of offsets.

This all would affect how I have to set up my post processor. I would have to define the G59 offset correctly in each post to ensure the router was on the table. It makes more sense to me, to set up the machine the way that I descirbed in 1-4 above.
It's best to assign the part origin to one of the work offsets. Your post processor should assume that the part on screen has the correct origin already set, and that all the dimensions are correct.

EDIT: Oops, you said case closed.

13. ## Thanks for the clarification

Hey Sniper,

Thank you for your clarification and educational discussion. I am starting to get a better feeling of what the offsets are for, what they do, and how to use them.

That is very helpful. I really appreciate you taking the time to set me straight.

I have no problem letting you have the last word.

R/Todd

14. Diamond
Join Date
Dec 2007
Location
Southeastern US
Posts
6,225
Post Thanks / Like
Likes (Given)
728
2589
Just to reinforce the answer, yes, industry standard is to do 1-4. The origin should always be a physically measurable position, (such as center or corner of a table) - when possible.

15. ## Excellent!

Thanks Tony.
I really appreciate your help with this.
I will set it up this way as soon as I get back to the shop.
R/Todd

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•