[howanc7]

Hi,

I am putting the MPU11 + GPIO4D + AC/DC, CNC11 version 3.12 system, on to an old Howa NC7 lathe. I am at the final setting stage and I am hoping people with more knowledge that me will help get past the last few hurdles.

The lathe has 6 micro switches for limits and home settings. I have the Z+/- and X +/- set and working, at the original positions. The original lathe had 2 more switchs to set the home position and I would like to re-use these. I wish the machine bed, to go first in a positive direction, until it makes the Z home switch, and then set to 150 mm. Then move the cross slide in the positive direction, until it makes the X home switch, and then set to 300 mm Dia. Idealy it would also move forward to the index pulse on each axis. Can anyone help me achieve this? Many thanks,

Cheers, Colin

[howanc7]

I guess what I am asking is; where do I connect my extra homing switches, and how do I change the Home File, so it looks for these, instead of the X & Z + limit switches? Colin

[cnckeith]

the limit switch hookup location are on the system schematic that is supplied with the kit and is online on the ajaxcnc.com website for download.
also here is a link to the tech bulletin page, each tech bulletin is a set on instruction on a specific topic. #22 is how to edit the home program.
Ajax Technical Bulletins | CNC Retrofit Control Systems for Milling machines, Routers and Lathes. Runs CENTROID Software
also, you will find a great deal of good information on the ajax user forum. search the forum for the subjects you are interested in.
here is the link. AjaxCNC Support Forum ? View forum - AjaxCNC Support Forum. NO LOGIN NEEDED
and often you'll get a faster response on the ajax forum for centroid related questions.

[cncsnw]

The system schematic will not show you where to connect separate home switches (the third switch on each axis) because separate home switches generally are not needed and not used. The Centroid control can home reliably using the limit switches, and that is what nearly every installation does.

If you want to connect your home switches, you can connect them to any otherwise-unused input points. But then you need to decide what you are going to do with them.

If the home switches are only a short distance in front of the limit switches, what utility do you expect to gain by homing to the home switches, instead of homing to the limit switches?

If the home switches are a considerable distance short of the limit switches (e.g. in the middle of travel), so you might hope to save time in the homing sequence by not having to go so far, what do you expect the machine to do if it is already past the home switches (to the plus side) when you initiate your homing sequence?

[howanc7]

Thanks for the replies; It is a large centre lathe and there is considerable distance to be saved by using the original limit switches. Being the wrong side of the limit switches would mean it would stop at the positive stop limits, I think, and it did that before with the old fanuc controler. The operator knows to jog to the negative sides of the home switches, before homing. I was hoping that there was a file that had the input numbers, that I could change to the new inputs that I use. Being a lathe, inputs 5&6 are not used.

I will look at topic 22 and keep reading, but appreciate any help I get imnensely, Thanks, Colin

[howanc7]

I had read Bulletin 22 before, now with more study, it seems that the home command operates an M92/Z, which jogs slowly (positive) to the Z +ve limit switch, stops, moves negative until the switch resets, and then continues on to the next index pulse, and stops. It then does an M26/Z setting Z at 0. Then repeats in X. Reading my manual on M (Macro) Functions it says that above M90, they can not be customised.

What I would like is to use is separate home switches, and set home to these home actual positions, +150 mm in Z and 300 mm diameter in X. As I have an off machine tool setter, and lots of tool holders, I could then do machining from these settings. Is there anything I can do? Cheers, Colin

[cncsnw]

M92 (and M91, for axes which home in the minus direction) goes to the home switch number specified on the Machine Configuration screen. The plus and minus home switch input numbers are usually the same as the plus and minus limit switch numbers, but they are not required to be.

If you wish, you can connect your home switches to INP5 and INP6. You would then enter 5 and 6 as the plus home switch input numbers for the respective axes. Then M92 would look for those switches.

You are correct that M92 would simply stop and cancel with an error if it ran into the plus limit switch while looking for a plus home switch on a different input. As long as the operator knows that it is his fault, not the control's, then he will get along fine.

As to what positions the DRO should display after it stops at the machine home position (that is, at the first index pulse to the minus side of the plus home switches), that depends upon whether you are talking about Machine Coordinates or about local (workpiece) coordinates.

Typically, the zero point in Machine coordinates (Machine Zero) is at the homed position.
Typically, the zero point for local (workpiece) coordinates is X at spindle centerline, Z at face of part, after applying any active tool offsets.
Typically, the position displayed on the DRO is a local position, relative to workpiece zero.
Unlike on some other controls, a Centroid control always has one or another workpiece coordinate system active.

If it makes you feel better to see Z150 X300 on the DRO as soon as it is done homing, you could set all your workpiece coordinate systems to Z150 X300 while the carriage is at machine home, with no tool offset applied. You would then use tool geometry offsets to make up the difference, to get any given tool from there to a measured position on a part. That is normal operation for the X axis. It is awkward for the Z axis, because it means that, if you program with Z0 at the free end of the part, then you have to re-measure all of your tools' Z offsets whenever you change to a different length part. If you are going to set your workpiece zero so that Z always shows 150mm at machine home, regardless of the length of the part in the chuck, then you will probably want to adopt the programming your parts from a Z0 that is at the chuck face.

If you can get used to the idea of seeing varying numbers on the DRO when the machine is back at machine home, depending upon the length of the current workpiece and the values of the currently-active tool offsets, then you can follow one of Centroid's recommended tool setting procedures, and you won't have to re-measure all your tools when the part length changes, even if you program from the face of the part. For example, procedure "1" or "1a" in the tutorial on my web site:
Lathe Tool Length Offsets Explained
If you prefer your method, use procedure "2", but instead of setting Z0 X100 in the one-time part zero, set Z150 X300.

[howanc7]

Thanks, I remember now that with the fanuc system it set X 0, Z 0 on the home switches. I then set my X to 300 mm diameter using G50, and as you say set my Z 0 by touching on the job and moving forward by the amount of facing I would do, again using the G50 command.

I will take your post to the machine and have a play. Will re-post how I get on. Regards, Colin

[howanc7]

Well, this problem seems fixed, it repeats to less than one micron in both Z and X, using the existing home switches, so I am very happy with this. Thanks, Colin