Hello Guest it is August 20, 2019, 02:07:47 AM

Author Topic: home sequence  (Read 9927 times)

0 Members and 1 Guest are viewing this topic.

Offline RICH

*
  • *
  •  7,351 7,351
    • View Profile
Re: home sequence
« Reply #10 on: March 11, 2012, 10:59:02 AM »
hmm.... 5 pages on G28 in the book, :) have a cup of coffee if you intend on waiting :D
RICH
Re: home sequence
« Reply #11 on: March 11, 2012, 11:02:34 AM »
OK,
BOTH axis words are required and it works as intended althought it says "All axis words are optional".
Re: home sequence
« Reply #12 on: March 11, 2012, 11:14:34 AM »
  If my HOME pos is Z0,X0 and I am currently at X2,Z-2 and want the tool to go to Z-1 before going home, program G28 Z-1 and there should be 2 moves.
Z will go to -1 THEN both axis will (should) go to HOME. I only get the first move.

Program  G28 Z-1 X2 and it does as described in the manual. An axis with NO move should not be required, imo and interpretation of the manual.

Used longer moves to clearly see in sim.
Z-30 X-2  =  Current pos.
G28 Z-2 X-2

Attached is from MILL GCodes.
« Last Edit: March 11, 2012, 11:50:20 AM by Overloaded »
Re: home sequence
« Reply #13 on: March 11, 2012, 11:35:29 AM »
Russ,
G28 and it should go home?
G28 X0.0 and it will home the x
G28 Z0.0 and it will home the z
G28 X0.0 Z0.0 and it will home both in a combination move
G28 X?.? Z?.? and it will home via the intermittant point defined

How's it suppose to work?
RICh

G28 and it should go home?                         Agreed, to the pre-programmed HOME position
G28 X0.0 and it will home the x    Disagree, X should go to the pre-programmed X0 position, followed by Z going to the pre-programmed Z0 position, no actual HOMING will take place.

G28 Z0.0 and it will home the z    Disagree,  (reverse of above)

G28 X0.0 Z0.0 and it will home both in a combination move   Disagree, G28 does not HOME (Ref) an axis, just sends to the pre-programmed HOME pos via X0,Z0 in this case. (X0,Z0 may or may not be the actual HOME pos.)

G28 X?.? Z?.? and it will home via the intermittant point defined  AGREED

Offline RICH

*
  • *
  •  7,351 7,351
    • View Profile
Re: home sequence
« Reply #14 on: March 11, 2012, 11:59:25 AM »
Still reading Russ,
G90 & G91 come into play and also if you have a part offset it makes a difference.
Maybe you will want to have breakfast also....... and yes what you have posted is true since its all about an intermediate step.
My bad on the description....  ;)
RICH


Offline RICH

*
  • *
  •  7,351 7,351
    • View Profile
Re: home sequence
« Reply #15 on: March 11, 2012, 12:37:52 PM »
Maybe you better eat dinner....... ;D
RICH
Re: home sequence
« Reply #16 on: March 11, 2012, 06:02:57 PM »
 :D
Goin' out to supper now, be back later tonight.
 ;D

Thanks,
Russ
 :)

Offline RICH

*
  • *
  •  7,351 7,351
    • View Profile
Re: home sequence
« Reply #17 on: March 11, 2012, 09:49:22 PM »
A few comments on wording which is important.
A machine has extreme travel limits. A point within the limits must be defined to the controller ( Mach3) so that all other movements can be associated. That point is machine zero and as such is known, fixed and defined. Home is just a point within the limits and it can be anywhere, but, home is usually machine zero. So home is used interchangeably with machine zero many times. Referencing is used to describe the condition where one has moved to some point and done something to tell the controller that the current position is machine zero or home. Homing can be done automatically, using the MDI, or manually and used to describe the motion of returning to machine zero. Fixture offsets are defined locations away from the home position. Fixture offsets are not to be confused with tool offsets. So an offset is just some distance from a point and needs to be always clarified. So much for the play on words!   

G30 - behaves the same as G28 and is unique as compared to G28. G28 is associated with the primary machine zero. G30 allows for machine movements to additional machine zero's and requires use of other parameters along with the G30 command like P or whatever. Mach's G30 use is not defined in the manuals other than "or just use G30".  So there is more to G30 and it's dialect of use may vary from manufacturer to manufacturer and can even be proprietary.

G28 intended use was to provide movement to an intermediate point before continuing on it's way to machine zero. It provided for eliminating some coding in a program and best example of use is to avoid an interference in the tools path to machine zero. G28 by itself is an incomplete command to some controllers but Mach ( and some other controllers ) provide for  movement without axis definitions resulting in a transverse move to machine zero. As noted in Mach definitions, the intermediate point is the current point and only one movement is made when no axis words are given, where as in Smid’s definition, one would need to add the current point / axis words as part of the G28 definition.  One must be careful in it's use since G90, G91, and additionally Fixture Offsets can affect the resulting machine movements when G28 is commanded. So it’s always interesting to see how different controllers use the commands but in the end the important definition is the one for the controller that is being used. 

Smid reference says:
G28 X0.0  “will only send the X axis to the X axis zero reference position”.
But as Smid points out the axis values associated with the G28 should always indicate an intermediate point and at least one axis must be specified.

In MACH Lathe:
G28 X0.0 - if a G54 / work offset exists and you are away from the exact offset value then you will have two movements. IE; it will first go to the intermediate value ( the work offset value ) and then go to X axis machine zero.

G28 X0.0 – if G54 exists and you are at the exact offset value then you will have one movement
ie; since your at the intermediate value there is no need to move to it so one move only to
to the X axis machine zero.

G28 X0.0 – if no offset exists there is no intermediate movement and the axis just goes to X axis machine zero.

G91 G28 X0.0 – there is no movement since mode is changed to incremental and the request is for zero movement

G28 – only one movement back to machine zero irrelevant if there is a work offset

All of the above is with tool zero / master tool but it’s worth going through the above with a call for a different tool. May as well try them with additional offsets.

RICH

Offline BR549

*
  •  6,886 6,886
    • View Profile
Re: home sequence
« Reply #18 on: March 11, 2012, 10:24:03 PM »
Rich you have the G28/G30 wrong for MACH3 it is NOT like Fanuc.

G28 takes you to the defined HOME value as set in config. An offset from the home switches
G30 takes you to the Machine Home as defined by the switches or you setting it manually

Just a thought, (;-) TP

Offline BR549

*
  •  6,886 6,886
    • View Profile
Re: home sequence
« Reply #19 on: March 11, 2012, 10:40:13 PM »
Also the command structure between the G28 and G30 is different.

(;-) TP