Adding a 4th Axis to the Oi Mate MC Control

[MaxWeber]

Yes those applications you reference tool changers, pallet changer are typical for that type of drive. A tool changer is basically an indexer, and true non-simultaneous. I assumed you didn't need that by the way you described it, i use the beta drives for these items and others.
Either way yes extensive ladder work needed.
I vote 3rd party.
Good luck!

Yeah I think that sounds like a fun project. I'd like to build an indexer with a high quality reduction gear (cross roller bearings?) and servo controlled by mach 3 software. The side effect would be saving a little cash too ;-)

[rodney247]

Indexer manufacturer

https://www.indexdesignscnc.com/

[MaxWeber]

Indexer manufacturer

https://www.indexdesignscnc.com/

Yes thanks for bumping this thread and checking in!

I basically went from having a good chunk of free time with my old job to almost zero free time with a new job about a month after I started this thread

So a homebrew 4th axis is out of the question, but the index designs 5th axis is now in play!

They use a standalone controller that has a number of options available for how it's run.

I'd like to keep running my programs natively from PCMCIA memory card (2GB) and send M code indexer signals via RS-232, but it sounds like I might not be able to split I/O between two channels like that. I saw some discussion on this forum about a potential set of parameters that could accomplish this, but I don't think they ever got it working. So that leaves me with running the entire program from the indexer controller and drip feeding my CNC from the serial port. It honestly sounds like a sub-optimal configuration, but am I just being biased against it? Does anyone else have an opinion about it?

[MaxWeber]

The parameters in question are:

0020 - I/O CHANNEL: Selection of an input/output device or selection of input
device in the foreground

0021 - Setting of the output device in the foreground

0022 - Setting of the input device in the background

0023 - Setting of the output device in the background

[MaxWeber]

Ok so I think what I mentioned above is correct. Here's a snippet from another forum where a user successfully tries to do what I want to do:

Success!

for anyone attempting this for themselves, i'll outline the params that need to be changed and post my code below.
This allows you to run your main program from the memory card (or another source) and communicate via com port with the indexer.

params
param:110 bit:0 must be 1 This separates the input and output channels, allowing you to use params 21-23
param:21 changed to channel 1 in macro then back to 4 at end. change this to suit.
param:6006 bit:0 must be 1 This allows use of logical expressions in your macro
param:6001 bit:1 must be 1 Leaves leading zeroes as zeroes (instead of a space)
param:6001 bit:4 must be 1 outputs CF after data output (for hardinge controller comms)
param:6001 bit:6 must be 1 Clear custom macro variables 100-149 on reset
param:3404 bit:6 must be 1 prevents end of record alarm when M99 is read

to set up the macro as an M code (I used M50)
1)in mdi mode press offset/settings button, then seting soft key, change parameter write=1
2)change param 3202 bit 4 to 0 to edit 9000 series programs
3)change parameter write back to 0, hit reset
4)if no program in o9020 spot, save program as o9020 in controller memory
5)change parameter write back to 1, then param 3202 bit 4 back to 1, locking 9000 series programs
6)change param 6080 to 50 (or whichever empty M code you are using)
7)change parameter write back to 0, locking parameters

and here's my final code:
when outputting zero with 3 digits before and after the decimal (required by the hardinge controller) you still get 0 (instead of 000.000), hence the homing condition instead of just outputting 000.000

code
(A MACRO TO SIMPLIFY THE USE OF A HARDINGE ROTARY INDEXER)
(CALLS AN 'S' ARGUMENT AS #19)
(USES FIXED ROTARY SPEED OF 300 DEG/SEC. PROGRAM USES ABSOLUTE ANGLES ONLY.)
(-----------------------------------------------)
(USER DEFINED VALUES)
(#19=S) (CALLED VARIABLE. SENT FROM MASTERCAM)
#101=4 (I/O CHANNEL YOURE STARTING FROM)
#102=1 (I/O CHANNEL THAT INDEXER IS CONNECTED TO)
(-----------------------------------------------)
#100=#19

IF[[#100LE360]AND[#100GE0]]GOTO10 (CHECK THAT ANGLE IS POSSIBLE)
#3000=101
N10

G10 L50 (NEW I/O CHANNEL)
N21 R#102
G11

POPEN (OPEN PORT)
DPRNT[] (CLEAR BUFFER)
G04 P64

IF[[#100EQ0]OR[#100EQ360]]GOTO25 (HOME)

DPRNT[XG090] (SET TO ABSOLUTE)
G04 P64
DPRNT[XF300.000] (SET FEEDRATE TO 300)
G04 P64
DPRNT[XS#100[33]] (SET ANGLE TO S ARG)
G04 P64
M12 (FIRE TRIGGER)
G04 P1500
M13 (CANCEL TRIGGER)
DPRNT[]
PCLOS (CLOSE PORT)

G10 L50 (SET IO CHANNEL TO ORIGINAL)
N20 R#101
G11

M99 (END SUBPROGRAM)

(-----------------------------------------------)
(IN CASE OF S=0)

N25

DPRNT[XG088] (GO HOME)
G04 P64
DPRNT[XF300.000] (SET FEEDRATE TO 300)
G04 P64
M12 (FIRE TRIGGER)
G04 P1500
M13 (CANCEL TRIGGER)
DPRNT[]
PCLOS (CLOSE PORT)

G10 L50 (SET IO CHANNEL TO ORIGINAL)
N21 R#101
G11

M99 (END OF SUBPROGRAM)

usage
simply call it as M50 S180 (or whichever angle you want) from within mastercam (i use manual input)

[rodney247]

Here is the manual for the Index Designs TR6 5 axis indexer how to comunicate withe the CNC https://f3fcdf07-1be3-4a20-ae27-66ec...3ef0409221.pdf

[rodney247]

TR6 Demo communicating with CNC

[MaxWeber]

Here is the manual for the Index Designs TR6 5 axis indexer how to comunicate withe the CNC https://f3fcdf07-1be3-4a20-ae27-66ec...3ef0409221.pdf

Thanks this is really helpful. You work for index designs? I've been talking with Bob about getting a TR-6 but since I'm a newbie to rotaries I wanted to make sure I knew what I was getting myself into. This document helps clarify things. By the way this manual describes the DNC to CNC process, it doesn't sound all that bad. As long as I'm not going to get a disruption in my current workflow (which has been working fine for years now) using fusion 360 CAM on my fanuc control. I see that the index control modifies the code whenever there's an A or B move, which sounds straightforward. I think I'll give the TR-6 a try as soon as I hear back from Sharp about the M code relays.

[oetkbyentc]

I haven't read all the replies but incase it hasn't been mentioned. Check parameter 110.0 It allows the setting of individual channels and devices for Input and Output. I have not used this under DNC with DPRINT but it sounds like what you need.

I'm not sure what you mean by "spare m-codes through RS232" unless you are referring to using an m-code to call a macro that has a dprint statement to send an ascii command code to the indexer.
Or possibly referring to the ascii command as an m-code?

[rodney247]

Max Weber Yes... and if you are in Southern Calif you can visit Index Designs and see the TR6 running usually on a machine making parts. Index Designs in located in Chatsworth. You can call ahead if you want to visit but it is not necessary. Best days would be Mon-Thurs