PDA

View Full Version : Work Offsets



RMT
08-17-2007, 04:39 PM
I finally got my Bridgeport Series 2 running, using Mach 3 Ver2.41 and I seem to have trouble setting the Work Offsets to zero.
I'm so used to not using offsets , I program the part to home in the upper left corner, and would like the machine to return to that from which it started, instead its going to machine home, at this point I have to hit stop and hit "go to z" and it returns to set up home, with the DRO's reading zero.
But when You hit "machine coord's" You basicly get the distance to machine home. So how does one set the "machine coord's" to zero at any place,
or better yet disable/remove the offsets all together.

Thanks for any help.

spoiledbrat
08-17-2007, 07:56 PM
typing "G92 X0 Y0 Z0" will set the current position to zero, without effecting the work offsets table.

typing "G28" will move your Z axis, then your X-Y axis(es?) to the G28 home position, which is set up in the Config_homing/limits options.

Be careful!

Rob

RMT
08-17-2007, 08:12 PM
I figured out now that G28 is what causes it to move to machine home
and replacing it with x0 y0 moves it to were i started and wanted to be.

Also discoverd disabeling the Home switches allows me to zero out the
Machine coord's, I feel this is a bug in the program.

You should be able to either disable offsets or zero machine coord's any
place on the machine, without added code to programs.

Thanks so much for the input, getting that beast running after sitting there for 5yrs makes me smile...

Frank

ger21
08-17-2007, 09:17 PM
I figured out now that G28 is what causes it to move to machine home
and replacing it with x0 y0 moves it to were i started and wanted to be.

Also discoverd disabeling the Home switches allows me to zero out the
Machine coord's, I feel this is a bug in the program.

You should be able to either disable offsets or zero machine coord's any
place on the machine, without added code to programs.

Thanks so much for the input, getting that beast running after sitting there for 5yrs makes me smile...

Frank

You can't change the machine coordinates because they represent the actual machines coordinates, in relation to the home switches. Mach's normal coordinate system is G54. You can zero the G54 offsets at any time by entering zero's in the offset DRO's on the offset page.

You can set an offset amount for your home switches so that when you home the machine, 0,0 is wherever you want it. Just put a value in the offset column under Config>Homing/Limits.

Also, the manual has a lot of info on explaining and using the coordinate systems.

RMT
08-18-2007, 11:13 AM
I guess I'm used to using the AHHA controle software, there having G28 at the end of program just seems to replace having to wrte x0 y0 , were in Mach 3 it will like you said take you to machine home.

Also I tried to type in the DRO , for one when the "Machine Coord" LED
is red i.e. its displaying the distance to machine home You can not type in
the DRO's , even after restting in config>fixtures and saving, yes all DRO's read zero in the offset page, yet my toolpath , because of G28 still shows movement to machine home, so when I went back to the offset page , click on machine coord's the far right DRO display again distance to machine home typing in zero just moves it over to the middle DRO's, I guess were You can save that offset for any selected G54, G55.... and so on. I read the instructions but had trouble following them, I must not be the only one since there seems to be a lot of confusion how to use these offsets.

Frank

Geof
08-18-2007, 12:02 PM
I guess I'm used to using the AHHA controle software, there having G28 at the end of program just seems to replace having to wrte x0 y0 , were in Mach 3 it will like you said take you to machine home.....

..... I must not be the only one since there seems to be a lot of confusion how to use these offsets. Frank

G code and CNC machine design has certain standards or conventions...but it seems not all software nor all machine designers follow them. This, I think, is why confusion sets in. In my opinion it is better to follow convention even if it does not seem logical; at least then everyone is on the same page.

Machine Home or Machine Zero is a fixed point which, from the operator's point of view, is in the right rear corner of the work area with the spindle as high as it can go. On a moving table machine the table moves forward and to the left when homing because that is what places the right rear corner under the spindle. On a moving gantry machine the gantry (X axis) moves to the right and the Y axis moves to the rear. All movement from machine home is measured in machine coordinates and is negative motion.

Because it may be inconvenient to program based on the location of the machine zero, i.e program in machine coordinates, it is possible to set Work Coordinates or Work Zeroes, that can be located anywhere within the work area. G54 is the first work coordinate and is the default option if there is no explicit command for a work coordinate in a program. Depending on the machine fifty or more work coordinates may be defined; the numbering of the first six is G54 to G59, the next six G110 to G115 and above that different machines use different numbering systems. When there are no values entered into the tables in the software for the work coordinates they are effectively the same as the machine coordinate system. Absolute programming using G90 defines positions within these coordinate systems; Incremental programming using G91 defines distance moved within these coordinate systems.

When using any work coordinate system the command G28 (just G28 no axis identification) instructs the machine to return straight to the home position. Depending on the machine this can be hazardous; some machines interpret this command on the Z axis first to pull the tool clear of everything and then home X and Y; some machines just go in a straight line from the position at which the G28 was commanded and if there is anything in the way of the tool a crash ensues. G28 can also have an axis designation so that only that axis homes, however, care is needed with this because in this case the machine will move, using the current work coordinate system, to the coordinate given for the axis and then go home. For instance if the tool is a the position Z1.0 clear of the work and the command G28 Z0. is given the machine will first move to Z0. which can result in a crash. To avoid this it is possible to include the incremental command G91 G28 Z0. to avoid the first motion; the incremental movement is zero.

Finally, for the this description, G53 is an overriding command. It does not matter what work coordinate system is active the command G53 instructs the machine to use the machine coordinate system for the move given in the instruction block including the G53. The block G53 G00 Z0. instructs the machine to take the Z axis to machine home by a rapid motion. Of course, any coordinate value can be used so it is possible with G53 to take the machine to a defined location.

RMT
08-18-2007, 07:28 PM
You right that machines are all different and suppose it is best to stick to convention, I don't claim to know all nor what is the best way of doing things, I'm just used to a certain way, the old bridgeport boss mills have machine home on front left side of the table, that might make it easy to change tools, but loading parts into the vise I preferred the back left side of the table as home, just behind or in line with the rear vise jaws.

So all the programs I write work of that point, don't really care where home on the machine is, just want to "home " the machine to that point, (stop mounted left side of the vise for x and back jaws for Y) put part in and run program.

In 7 years running the AHHA control not once did I home the machine, this is a stepper motor slow as mollassis machine.

This is probably one reason why most people buy the same make of machine, because they get used to the control and don't want start over
learning the control.

I apreciate You clearifing things for me since I obviously don't understand all the G codes, quess I'm too busy making chips than to worry whether G28 should take the machine to X0 Y0 or to machine absolute home per convention.

Maybe one more thought hitting "Go to Z" in Mach 3 shoudn't it raise z first on a milling machine and how do change it, because now it moves x and y before z, which is bad..

Thanks Again
Frank

ger21
08-18-2007, 09:40 PM
Maybe one more thought hitting "Go to Z" in Mach 3 shoudn't it raise z first on a milling machine and how do change it, because now it moves x and y before z, which is bad..

Thanks Again
Frank

set a "Safe Z" height and turn on "Safe Z" under Config>Safe Z setup.

RMT
08-20-2007, 07:04 PM
After setting safe z hight , when hitting "go to z" the z axis lifts first and than
moves x y..... this is great, things starting to work the way they should.

Thanks everyone for pointing me in the right direction

Frank

corrie
12-13-2008, 11:59 AM
Hello I,m not sure how to use the work offset screen,maybe someone can explain it to me.Typicly after i set my wood in place and lock it down I manualy jog to the start position and zero all axes before starting the run.i would like to know how to set up the offset from my home position .This way when doing a roughing pass and then a finish pass I,ll be sure to know the start point remains the same for both programs.After homing the machine, do i jog over to where i want to start ,then re-zero all axes and call that offset 1.Just a little confused on the work around any help woud be appreciated and where to find some writen material for mach3,thanks in advance.

9lrac9
12-13-2008, 01:38 PM
Corrie... 9lrac9 Here, you can go to machsupport and download a PDF Mach3 manual about 150 pages, is is worth the time and paper. And as to your problem with offsets, I went nuts with that too. I am not a programmer, and I have been a manual guy all my life, and now with all these buttons and offsets and all the rest of what it takes to make a part. I am ok now except for the scare on my forehead form banging my head on the wall. I have got alot of info from the CNC zone and there is alot of good helpers on this site. I zero my machine at machine home, then I go to where I want the part to start XYZ zero them at your part and then zero on your run screen go to offset page and the lower right corner to save offsets click to open and you will see your part home or part zero not machine home or machine zero. Run your part and when its done on your run screen push reference to home Z will retract first then y then x and they will go to machine home. Or MDI G28 All will go home. Hope this is not to long winded for you as I almost go rid off my machime over this problem. Mastercam and Mach don't like G28 M/C PUTS G28 at the begining and I did not pick it up in the Gcode and Mach always after setting part zero sent the program back to machine home and tried to run the part from there and when it could not the machine would stop. And I did not understand. and do I now understand. I had to edit all my programs and rid them of G28.

corrie
12-13-2008, 03:05 PM
Thank you very much for the info.I had kinda thought the procedure went that way,but after the program ends and I reference back to machine home,what do I do to make it go back to machine part zero.? Do I give the machine a run command back to machine part zero?How do I call for the offset agian from machine zero,sorry if I,m confusing the issue.I will check out the PDF,thanks agian.

CNC Viking
12-14-2008, 07:44 AM
Geof,
Great post on Coordinate homing G-codes:cheers:
I am just learning to set up my Mits Meldas 520 control, and I must say that their Manuals are not always very clear in explaining the various functions of G-codes, M codes etc. Many times one have to check elsewhere just to fully understand and/or have ones understanding of the text confirmed.





Mastercam and Mach don't like G28 M/C PUTS G28 at the begining and I did not pick it up in the Gcode and Mach always after setting part zero sent the program back to machine home and tried to run the part from there and when it could not the machine would stop. And I did not understand. and do I now understand. I had to edit all my programs and rid them of G28.

9lrac9,
Is that a precautious step by MC's post? Can you not tweek the post to drop the G28?

CNC Viking
12-14-2008, 09:03 AM
Mits Meldas 520 Manual's page for G28, G29.

How do you understand that?

9lrac9
12-14-2008, 10:49 AM
Geof... I went to a different post processor not the Mfan that most use as this one is in, I and J and it drops the G28 from the post on the start up lines of the program. I am still a new guy to cnc and I program from part zero not from machine zero. I scraped some expensive material thinking that it was ok and walked a way for a mimute and I came back !@#$%^&*() what was I thinking to walk away from a cnc and a new one at that and I did not understand the whole picture yet. I have never made that mistake again...

9lrac9