[StarAppJohnUK]

I have been wondering if its possible to make two separate parts out of the same bar one after the other, switching from one program to the other automatically/within the program. The reason I am thinking about trying this is because the two different parts need a unique sequential part number and date of manufacture engraved on them per pair of parts. It's compulsory that the parts are made out of the same batch of material

Usually there isn't a machine available for a long enough period of time to make one of the parts individually at the same time, so by making the two different parts at the same time, I'm hoping to reduce the time pressure I have to have completed pair of parts if I only have the one machine spare when the job comes up.

It's a fine margin at times when the boss tell me to put these particular jobs on as I currently have to run 50 of the one part, reset the count, and then make the other 50 parts etc to keep on top of the 'pairs'. If I scrap any of the first part I can run out of material for the second part and then not have the full quantity of 'pairs'. My boss is an arse who always replies with 'I don't care about your excuses, I only care about the figures' if I run out of material, cock up the count, or the 'pair count' is too little when the customer calls for a part delivery. this way I'm hoping it will be easier to manage and have a steady flow of pairs and get my boss off my case.

The two jobs can be tool set for each part and picked up with the same sub spindle collet size, I just don't know how to flit between them. I have the engraving macros for date and part count. I'm hoping to do this on a 32i fanuc control on a star SR32J.

If its possible, if someone could provide a template/instructions on how to go about this I would be very grateful.

thank you

[handlewanker]

So....my two pennoth worth as I'm a newby at G coding.......you have two separate parts to be machined on the same bar stock material......for example.......a 25mm steel square bar billet in a vice, sitting down on parallels, and you have two separate programs, one for each part.

You could create a new program in Notepad by pasting each one in, one after the other, and start each program with G54....G55 at the beginning to make the tool go to the respective part at the start of each program.

This way you end up with one long program in place of two programs.........the second program has the G55 edited in at the beginning to position the tool for the second part.

I assume you are working with an auto tool changer and not stopping mid cycle to manually change over tooling etc.

This is only a suggestion as I'm learning G coding sequence and if it's totally nonsense..... I learn too as to how it can be done.
Ian.

[RCaffin]

Ian is almost there.
You need a top-level program which calls a subroutine 50 times (or whatever number) with M98.
The subroutine contains two M98 calls to other subroutines, one after another. Those two subs are the programs you have now, suitably edited.
That way you call your two programs as pairs.
You will need to look up subroutines in g-code, but they are really simple - and really powerful.

Cheers
Roger

[handlewanker]

Hi Rog....sub routines are beyond my ken.......I don't think my system will cater for subs anyway that's why I went the simple path......the G54 series is so powerful and easy to understand.....I have to wonder if it would work as I might need to do something similar one day......BTW...compliments of the season.
Ian.

[RCaffin]

Hi Ian
Never say never ... :-)

What control SW are you running? If it is Mach3, I can assure you it does support subroutines. UCCNC, LinuxCNC, Fanuc: they do too. Most control SW will - it's the CAM which often cannot handle the idea.
Yes, G54 could be part of the solution, to be sure, although there are other ways as well.

And a Happy New Year to you and all.
Roger

[warrenb]

I'm lazy. Since I don't do much production work and you're cutting only 50 part sets a I would just make a single toolpath with the parts and run your engraving macro separately. By the time I had all the subroutines programmed and proofed I would be half way done a lot of 50 part sets.

[RCaffin]

Hi Warren

Yes, I could agree, except that it seems that OP makes these in JOB LOTS of 50 at a time. Once the code is written and checked, subsequent runs are just so easy.

Cheers
Roger

[StarAppJohnUK]

Hi all

Thank you all for the replies so far, just to clarify im going to try to do this on a 32i fanuc control on a SR32J star sliding head machine. I am currently only running on parts 50 at a time to keep on top of pairs completed in a day. The whole order is 1000 'pairs'. I currently run 50 part A, change to part B run 50 etc..I want to be able to do machine 1 of part A then machine part B, so I have completed pair quicker.

It's looking like m98 sub routines is the way to go, which will be fine on Head 1. Its just working on the sub spindle that is going to be awkward to set the Z geometry for the different parts, depending on how much is sticking out of the sub spindle on the 32i control.

If the amount sticking out at the end of the spindle is the same for each part, then I could get away with working with the same Z geometry offset. X is X so it doesn't matter as I don't need to change that all.

If I was doing this on an 18i Fanuc I could set a different G50 Z value for the sub spindle and I wouldn't have a problem I don't think. It's just this 32i Control uses a G132 code (ZB axis work coordinate) and I don't how to set the different z geometry offset for the different tools depending on how much is sticking out the sub spindle. you set the tool in a similar way to G50 Z method, but you minus the part sticking out the sub spindle and press measure when you are at the cutting point of each tool.

I could be miles away and over complicating it, but could I use #2601 variable somehow? ( z work coordinate shift amount) Im not entirely confident in using system variables yet.

I suppose I could also try using g50 z value on this 32i control and see if it works too, don't know why ive never tried it before. The G50 Z value is the distance from the reference position when the tool is called, to end of the cutting tool.

thanks again,

[RCaffin]

I don't have a Swiss lathe, just a VMC with a horizontal lathe chuck. But what I do might work for you, sort of.

I am machining a long thin needle valve. I can't machine it all in one hit because of deflection - the machine does not have a tailstock. By starting with some 10 mm 2011 alloy, I can machine the 'active' part of the needle valve in one op (~30 mm long). Then I move the main tool out by 20 mm and stop the chuck. I loosen the chuck and move the workpiece 20 mm out until the tip touches the tool, and retighten the chuck. Press go and the lathe machines the long thin handle behind the 'active' bit.

Yes, this requires some custom programming, but it works - very well. I don't bother with any G54 commands: I do the maths on paper and write the code to handle the offset. Typically I am machining to 0.01 - 0.02 mm.

Yes, this means I have to stop the chuck half way through and move the workpiece, and it means the handle or shaft may be a few 10s of microns offset from the body of the needle due to tolerances in the chuck jaws and irregularities in the Al rod - but that seriously does not matter.

HTH
Cheers
Roger

[gizmo_454]

If the parts are required in pairs, you could theoretically combine the 2 programs into 1 and make both parts with one program. That would keep them paired up perfectly, so long as none of them get scrapped. The other option, mentioned above, using the subprograms, would probably be the better way to go, that way, you can call one, then call the other. My only concern with using the sub programs would be keeping all of the wait codes lined up and straight.

I think I would, personally, choose to write it as 1 program that does both parts. Then all wait codes can be lined up properly and without issue. Depending on how long the parts are, you could more than likely do them both with 1 chucking of the main. And as for the different part length stick-out of the sub, you could mathematically determine the difference and call a G50 W value to offset the sub's Z axis from where the first part was setup. Just remember to cancel the G50 shift when you are done using it. Again, personally, I would turn it on at the start of a process with a given tool and then turn it off before calling the next tool. That way, if you have to stop after a tool for some reason, you don't have to worry about having to go to MDI to cancel it. Also, doing it in one program, you could even possibly write the program using CAD/CAM software since it would be just straight code without sub programs.

The Fanuc 32i is a powerful control. We have the 32i model B in our Tsugami and, despite some pet peeves regarding the quirkyness of it, it does a fine job. Good luck to you! And let us know how whatever you decide to do works out!

Mike

[MCImes]

This is silly easy.

1. Load both programs in your control, run neither of them independently, as they will be run as sub programs by the following master program
2. create a master program that is 3 lines:
M98 P0001 (run part 1 program)
M98 P0002 (run part 2 program)
M30 (repeat)
3. Run the Master Program and create a pair of parts.

I used this exact same code for a customer of mine that wanted to run 2 different parts, every other cycle, as their production demand was equal for both parts but they did not want to run separate batches of parts as production was hand-to-mouth at the time. It worked great.

(the M98 Pxxxx call will likely be a different program number than 1 or 2. Just substitute the xxxx with your 4 digit program number for each part program)

Note, if the parts are different length and you have to input the part length into your barfeeder, you will have to enter the longer of the 2 parts

Edit: In regard to the different sub spindle stick out lengths, I would probably just use different geometry offests in the slave program (I would just call the 2nd program run the 'slave program'). For example, one program could use offsets 1-50 and the other 51-100. Then, to reduce operator error, I would make the 1-50 offsets the 'master'. I would only apply offsets to offsets 1-50. forget 51-100 exist at all. Then, at the beginning of each tool block in the Slave program, use a macro statement that writes the offset and geometry from 1-50 to the corresponding 51-100 offset. This sounds complicated and scary but is actually very easy. It would only take a few lines of code, like #2751=#2701; #2151=#2101; and so on. You would have to write macro statements for each axis offset (X,Y,Z,R,T) for both wear and geometry, so you would potentially need up to 8 lines of system macro code at the top of each tool block in the program with slave offsets, but you would only have to do it once and its not as hard as you think.

I cant attach a more detailed explanation at the moment, but message me if you'd like more information on how to use system macros to copy tool geometry to a secondary offset.

Cheers!

[RCaffin]

Perzackly
Cheers
Roger

[StarAppJohnUK]

This is silly easy.

1. Load both programs in your control, run neither of them independently, as they will be run as sub programs by the following master program
2. create a master program that is 3 lines:
M98 P0001 (run part 1 program)
M98 P0002 (run part 2 program)
M30 (repeat)
3. Run the Master Program and create a pair of parts.

I used this exact same code for a customer of mine that wanted to run 2 different parts, every other cycle, as their production demand was equal for both parts but they did not want to run separate batches of parts as production was hand-to-mouth at the time. It worked great.

(the M98 Pxxxx call will likely be a different program number than 1 or 2. Just substitute the xxxx with your 4 digit program number for each part program)

Note, if the parts are different length and you have to input the part length into your barfeeder, you will have to enter the longer of the 2 parts

Edit: In regard to the different sub spindle stick out lengths, I would probably just use different geometry offests in the slave program (I would just call the 2nd program run the 'slave program'). For example, one program could use offsets 1-50 and the other 51-100. Then, to reduce operator error, I would make the 1-50 offsets the 'master'. I would only apply offsets to offsets 1-50. forget 51-100 exist at all. Then, at the beginning of each tool block in the Slave program, use a macro statement that writes the offset and geometry from 1-50 to the corresponding 51-100 offset. This sounds complicated and scary but is actually very easy. It would only take a few lines of code, like #2751=#2701; #2151=#2101; and so on. You would have to write macro statements for each axis offset (X,Y,Z,R,T) for both wear and geometry, so you would potentially need up to 8 lines of system macro code at the top of each tool block in the program with slave offsets, but you would only have to do it once and its not as hard as you think.

I cant attach a more detailed explanation at the moment, but message me if you'd like more information on how to use system macros to copy tool geometry to a secondary offset.

Cheers!

thank you for all your replies, I managed to complete the problem by following the method above. Although the only thing different to the above method, was i used the G265 (tool geometry input) code to set geometries on the sub spindle to solve the issue of differing part lengths sticking out of the sub, so I didn't need to use system variables, although it would've have been good to try out if I understood it better.

thanks all