Where is Home XYZ000 Supposed to be located on a Mill?

[countryguy]

Gang, I'm sitting w/ my Son and we're banging away hour after hour trying to setup Mach3 and our Mill. Sorry in advance for all the Q's but we are trying hard here. It's purchased used (yeah, I know I know). But I am OK w/ sweat equity and solving others mistakes. And there have been some doozies.

Where is a Mill tables Machine Home (000) supposed to be? I'm trying to load and tell Mach the home based on the switches as follows:

FROM THE FRONT OF THE MACHINE . Standing facing it.
X is to the far Right. (run length of 14.2")
Y has the table coming back at you to hit the limit switch (run length of 11.5")


Thanks

 

[Ray C]

Gang, I'm sitting w/ my Son and we're banging away hour after hour trying to setup Mach3 and our Mill. Sorry in advance for all the Q's but we are trying hard here. It's purchased used (yeah, I know I know). But I am OK w/ sweat equity and solving others mistakes. And there have been some doozies.

Where is a Mill tables Machine Home (000) supposed to be? I'm trying to load and tell Mach the home based on the switches as follows:

FROM THE FRONT OF THE MACHINE . Standing facing it.
X is to the far Right. (run length of 14.2")
Y has the table coming back at you to hit the limit switch (run length of 11.5")

Thanks

Try downloading the instruction sheet I created for the PM45 mill. It shows how to do it for that machine. See Post 24. http://www.hobby-machinist.com/showthread.php?t=21179

Also, there is no "standard" location for home. It's all relative to what you want.


Ray

 

[countryguy]

Thanks Ray.... Ever go by RayRay? LOL ;-) I found this as well on the Net. (everything there is true right) . I've seen Hood around and he's big into Mach3 and Home/Limit q's.

WE'll I have something wrong since Mach3 indicates the wrong layout so if I can use anything I wish, then I need to appropriatly setup the softmin max.. . Moving now and resetting.

Hood:
Table fully right means tool fully left in relation to work and that is X0 (Machine Coords)
Table fully towards column means tool fully towards you in relation to work piece so that is Y0
Head fully up is tool fully up and that is Z Zero.

Try downloading the instruction sheet I created for the PM45 mill. It shows how to do it for that machine. See Post 24. http://www.hobby-machinist.com/showthread.php?t=21179

Also, there is no "standard" location for home. It's all relative to what you want.


Ray

 

[JimDawson]

The way I normally set things up is to set X & Y 0 at an extreme corner of the work and Z 0 at the work top surface. I typically use the upper right corner as you are standing in front of the machine so that all of the moves into the work are in the negative direction. -X, the table moves right, -Y, the table moves toward the column, -Z, the quill moves down. It keeps me from getting confused, and also allows setting to the stationary vice jaw if you are using a vice to hold the work. When I create the G-code in the cam program, I move the part into the lower left quadrant. There a few cases that I use the work center for 000, but not often.

As Ray stated, there is no standard location. You just need to make sure that any move will not exceed the machine travel limits.

 

[DMS]

As others have said, there is no "standard" location. I have mine set to roughly the middle of travel for X and Y (9x42 BPT clone), and at the top of the Z.

Keep in mind I don't have much experience with Mach, I have only used LinuxCNC, but as far as home/limit switches, I think the following behavior is pretty common.

On my machine, I place the home switch wherever I want, and then I tell the machine that home represents some value. I have called all of mine "0", but I could just have easily said they were 5.334". With LinuxCNC you can also tell it to go to a certain position after hitting home, so on my Z, I drop down by 0.5" after hitting the Z home because I am sharing a home and limit switch on Z.

One thing that you may not have learned yet (and the reason why the exact location doesn't matter) is that there a number of different "zero" points. What you are talking about is called the "machine zero". I never, ever (well, mostly never) use the machine zero for anything. Before machining a part I will set a relative zero on the stock by touching off. The machine will remember this point (it's relative to machine zero) even after you power down. So don't sweat the location of the home switches too much, just make sure they work reliably and everything else works out in the software.

 

[John Hasler]

Is there a standard handedness? Sounds like countryguy is describing a left-handed coordinate system while JimDawson is describing a right-handed one.

 

[Ray C]

Most of the tutorials I've seen describe it as though you're looking at a map and use N, S, E, W to describe the origin of the table and/or piece coordinate system.

Most of the Mach 3 tutorials put the origin at the S-W corner of the table from the perspective of you standing in front and looking down at it.

----------------------
!------------------- !
!--------------------!
x------------------- !

The "x" would be the table origin of a S-W coordinate system and this is how I generally do things. In terms of the part, I tend to put the part origin on the S-W corner of a square item and use the center of a cylindrical item. -Just my preferences but, it really makes no difference.

I have two vises on the table right now and have G55 and G56 setup at each vise and when I put a part in there, I set a local origin for the part itself. G54 is the table home (i.e. "x") position. Just remember when you have multiple vises to make sure that each home (wherever it may be defined) has a safe Z level to not crash into anything.

Ray

 

[countryguy]

COORDINATE Systems and Onward Ho' Was: Where is Home XYZ000 Supposed to be located on a Mill?

Thank guys!! I really appreciate this forum as the "Friendly place" Much happier here than some others I experienced! TIA!!!!

That said;
I found several options and methods. Most work if you can get the machine and your brain to sync! I did figure out my issues in Mach3 and am aligning just fine now on what is Table Work 000(XZ) -vs- Machine HOME and relevant offset to 000 with the Home switches! Simply click ZERO XYZ and REGEN when I've positioned myself. What I need are two more switches! X++ and a Y++ I'll put Home in the middle and use this coordinate system. the best tip of my day today was that you think in terms of TOOL MOTION. Not table. Kewl!

This is a really nice website Ya'll (yes I put in Ya'll ;-) I am from Michigan but work w/ a lot of folk from OH and KY Anyway, I digress!
The Site: http://www.hsmworks.com/docs/cncbook/en/#Ch04_VMCMachineMotion

The statement:
when working with a CNC, always think, work, and write CNC programs in terms of tool motion, not table motion.
For example, increasing +X coordinate values move the tool right in relation to the table (though the table actually moves left).
Likewise, increasing +Y coordinate values move the tool towards the back of the machine (the table moves towards the operator).
Increasing +Z commands move the tool up (away from the table).





Thank a Ton RC.
So that X in this Drawing is the ToolBit location right? This is what I have setup now. (man I hope anyway). I'm unsure how to really emulate the "soft limits" for X++ and Y++ now. I have Home and zero points and a frame of reference. I'm so close!!! I'll read about "softl limits and what "emulation does later. I did input G55 and a fixture loc too. Very nice! MAn I want a PM-45 CNC setup I may just need to get this running smooth and sell it for one. Those Pics and your Setup doc are awesome! Love what your doing guys.
JJ

Most of the tutorials I've seen describe it as though you're looking at a map and use N, S, E, W to describe the origin of the table and/or piece coordinate system.

Most of the Mach 3 tutorials put the origin at the S-W corner of the table from the perspective of you standing in front and looking down at it.

----------------------
!------------------- !
!--------------------!
x------------------- !

The "x" would be the table origin of a S-W coordinate system and this is how I generally do things. In terms of the part, I tend to put the part origin on the S-W corner of a square item and use the center of a cylindrical item. -Just my preferences but, it really makes no difference.

I have two vises on the table right now and have G55 and G56 setup at each vise and when I put a part in there, I set a local origin for the part itself. G54 is the table home (i.e. "x") position. Just remember when you have multiple vises to make sure that each home (wherever it may be defined) has a safe Z level to not crash into anything.

Ray

 

[Ray C]

Re: COORDINATE Systems and Onward Ho' Was: Where is Home XYZ000 Supposed to be located on a Mill?

Thank guys!! I really appreciate this forum as the "Friendly place" Much happier here than some others I experienced! TIA!!!!

That said;
I found several options and methods. Most work if you can get the machine and your brain to sync! I did figure out my issues in Mach3 and am aligning just fine now on what is Table Work 000(XZ) -vs- Machine HOME and relevant offset to 000 with the Home switches! Simply click ZERO XYZ and REGEN when I've positioned myself. What I need are two more switches! X++ and a Y++ I'll put Home in the middle and use this coordinate system. the best tip of my day today was that you think in terms of TOOL MOTION. Not table. Kewl!

This is a really nice website Ya'll (yes I put in Ya'll ;-) I am from Michigan but work w/ a lot of folk from OH and KY Anyway, I digress!
The Site: http://www.hsmworks.com/docs/cncbook/en/#Ch04_VMCMachineMotion

The statement:
when working with a CNC, always think, work, and write CNC programs in terms of tool motion, not table motion.
For example, increasing +X coordinate values move the tool right in relation to the table (though the table actually moves left).
Likewise, increasing +Y coordinate values move the tool towards the back of the machine (the table moves towards the operator).
Increasing +Z commands move the tool up (away from the table).

View attachment 76533



Thank a Ton RC.
So that X in this Drawing is the ToolBit location right? This is what I have setup now. (man I hope anyway). I'm unsure how to really emulate the "soft limits" for X++ and Y++ now. I have Home and zero points and a frame of reference. I'm so close!!! I'll read about "softl limits and what "emulation does later. I did input G55 and a fixture loc too. Very nice! MAn I want a PM-45 CNC setup I may just need to get this running smooth and sell it for one. Those Pics and your Setup doc are awesome! Love what your doing guys.
JJ

Thanks for the kind words...

Yes the 'X' is the home location for the table. This is usually called "Machine Home". It moves to the S-W corner and the spindle moves to the highest location as defined by the home switches.

If you read that instruction sheet on homing, it should describe how to set soft limits. The values you enter will need to be commensurate with your table dimensions. Does your machine have limit switches as well as home switches? If you don't have limit switches, you need to rely on properly defined soft limits. FWIW, I use soft limits that are defined about 1/8" short of my physical limit switches as, when you physically trigger a limit switch, it throws a reset and Mach stops all operations. When hitting a soft limit, Mach stops but, does not need to get fully reset to start-up again.


Ray

 

[JimDawson]

Re: COORDINATE Systems and Onward Ho' Was: Where is Home XYZ000 Supposed to be located on a Mill?

The statement:
when working with a CNC, always think, work, and write CNC programs in terms of tool motion, not table motion.
For example, increasing +X coordinate values move the tool right in relation to the table (though the table actually moves left).
Likewise, increasing +Y coordinate values move the tool towards the back of the machine (the table moves towards the operator).
Increasing +Z commands move the tool up (away from the table).

Looks like I have been doing it backwards all this time, but I guess I'm not going to change now.:thinking: I might have to if I ever decide to start selling my controller software.