[MikieD]

We have a SKT21LMS with Oi-tC controls. In order for the tools to index, the X and B needs to be in the home position. Is there a way to disable this? We could really shave some time off if so. It seems ill conceived that it is like this anyways. You can still crash a tool (depending on tool used) into the main spindle in the home X position during a tool change and can crash the entire turrent into the B so I don't understand the point of restricting the X and B axis position for tool change... We have a job coming up and if we have to return X and B (especially) to the home position for tool change it will totally change how we want to run the part and triple cycle time or more. Being able to index where we want will shave a lot of wasted motion from our other parts as well. Any help appreciated. Thanks.

[gilchapa]

Those kinds of restrictions on the machine tool are usually programmed in the PMC. Have you checked the keep relay options of the machine?

[MikieD]

I'm not sure what to look for to disable it. Is what I'm wanting to do something that is common. I ran many google searches but found nothing similar. I would think it can be done though. What if you needed to turn a long skinny part that needed support from each side to prevent whipping? The way the machine is right now you would have to open chuck on the B, home B, tool change, back with B, and close chuck for each operation. That isn't very efficent at all.

[MikieD]

Does anyone know if you can enable multiple M-codes per line like other Fanuc controls? It is an Oi-tC. Thanks.

[MikieD]

Does anyone know if you can enable multiple M-codes per line like other Fanuc controls? It is an Oi-tC. Thanks.

I found the answer to this the Oi-tC can take 3 m-codes per block. Nice... Still no luck findin an answer on disabling a tool change only from x and b's home.

[MikieD]

I found the answer to this the Oi-tC can take 3 m-codes per block. Nice... Still no luck findin an answer on disabling a tool change only from x and b's home.

I changed the parameter to allow multiple m-codes. I gave it a try in a program with a few unconflicting m-codes. It didn't give a multiple address alarm like it would have done before but it was only reading and executing the first m-code in the block and skipping the others without executing them. Am I missing something? The fanuc manual said this ability was machine builder dependent. It said the same about a few other things such as a spindle command and axis movement in the same block as well as a tool change and spindle command. The skt21lms does both of those at the same time so I'm surprised it wasn't executing the multiple m-codes per block...

Still no luck finding an answer on making a tool change away from X and B's home position. I find it hard to believe that no one else is doing this or atleast wants to. Returning all the way home for the turret to index is such a waste of time and movement and totally inefficient. I pull up nothing, even with generic non machine specific, Internet searches... I can't be the only person wanting to remove the wasted time and movement. I can't be the only person wanting to remain chucked up on both ends of the part with multiple tools needed to cut the part and not have to unchuck a side and go home to change tools and come back and rechuck. Or can I? Starting to wonder if that is just something people accept as there is no mention anywhere and no one here has even responded to the subject with anything of use or even a desire to do the same. Is this something you can do on this machine or any machine for that matter? How do some of you turn parts that need chucked from both side for rigidity and need to use multiple tools on the part? Thanks.

[gilchapa]

Do not despair! It takes a little patience to fix a machine. Check the PMC and try to find a bit in the tool change ladder that checks for a position in the X and Z axes, that is most likely the lock, bypass it or erase it, restart the control and try again a tool change.

If it is a 0i you can change the ladder in the control itself.

Good Luck!

P.S. Im assuming that you have the manuals for this controller, if you dont PM me you email and i will mail them to you.

[MikieD]

Gilchapa, Thanks! I do have all the manuals. Would it be in the yellow fanuc parameter manual? If you have an electronic copy that would be great too though. I could keep a copy at home and on my phone. I'd love to look tonight for it too and my manuals are at the shop.

Do you know anything about the multiple m-codes per line? I found the parameter listed in the operator's manual. Is the ladder the 8 definable units that was listed beside the m-code parameter (3404)? The operator's manual said "Up to 3 M codes can be specified together in a single block when Bit 7 (M3B) of parameter No. 3404 is set to 1." Bit 7 was actually the first block of the 8. Is there possibly another parameter to read all the m codes and bit 7 just allows the m codes in the same block?

I'll PM my email and a big thanks again!

[gilchapa]

MikieD> Yes, that was the manual I was talking about (B64310), as that manual says, Parameter 3404 is the only one that affects the multiple M code execution. It may be that the M codes you are trying to input are preventing buffering (and therefore are not processed), see parameters 3411 to 3432.

[gilchapa]

MikieD:

Did you get this to work?

[MikieD]

MikieD:

Did you get this to work?

I tried it again and still no luck with multiple m codes. I tried to enter some of the m codes into the 3411 - ... parameters. It still would only read and execute the first m code in the block and skip the others. At this point have stopped looking into a solution.

I also don't know where to look for the ladder that holds the coding that prevents tool changes away from x and b home. I spoke with the service tech of the company I bought the machine from and he said that Hyundai would have to rewrite the ladder for me. I haven't checked any further on this either. It seems like it would be as simple as removing a line of code that looks for the mechanical switch showing x and b are home. I have spent a lot of time trying to improve the operation for my application but not having any luck.

I do appreciate you trying to help me.

[gilchapa]

Yes! It is simple as that, you can add a keep relay, for example K90.0 and bypass the requierement for the tool change to be on a fixed position.
Do you have the tools to do this? You will need the FApt ladder software, and a PCMCIA Card. If you have the PMC file and are able to send it over email I can look at it and modify it in my company, then you can load it onto the controller and try the tool change and if it doesnt work you can just change to your old PMC program.

[gilchapa]

My email address is [email protected]

[MikieD]

Yes! It is simple as that, you can add a keep relay, for example K90.0 and bypass the requierement for the tool change to be on a fixed position.
Do you have the tools to do this? You will need the FApt ladder software, and a PCMCIA Card. If you have the PMC file and are able to send it over email I can look at it and modify it in my company, then you can load it onto the controller and try the tool change and if it doesnt work you can just change to your old PMC program.

I do have a card. I'm not sure if the FApt ladder software is the software from the machine or a software to manipulate the machines software. I have never extracted anything from them machine before myself and not quite sure how to but do want to learn. I know stuff is on the card too. I'm not sure what but want to protect it. I am just learning about programming and machining. I had to fire the programmer/machinest/cad designer due to poor attitude and many other quirks... After gettin a few one on one days of training I quickly found out the past employee was not very good at programming either. With what I learned I expanded on and now have what was a 7 minute part down to 2:15! I can remove about 20 to 30 more seconds from the part if I could stop the homing for tool changes, use multiple M codes, and a couple custom tools that cut a chamfer at the same time as milling and drilling.

I know the guy I had did extract programs and made text documents on our computer. Can I just copy the PMC (is that the ladder) to the card, then to a computer, modify it and reload the CNC? Or do I need a certain software for my computer? I do have CAM software if that helps. If I can just load onto a computer I am still nervous I might wipe the machine and my programs out. I need to learn for just that reason though, so I can back everything up...

Do you min explain the keep relays more? I can't find a good definition or understandable example I can follow. What do they do exactly? could you break down what K90.0 means?

[jvangelder]

You can do toolchanges at G30 reference points as well.

I do tool changes at G30 W0 U0 while the B axis is usually just left at G28 B0. On our 21LMS the G30 locations puts the tool changer around x0 z8 off the chuck, works great for just about any program.

You can change the G30 locations by enabling PWE and the locations are around parameter 1500 iirc (no book in fornt of me)

No ladder rewrite, service tech needed, you can edit this in 30sec standing at the machine.

Be forwarned however, from my experence, you can set the G30's to locations that will cause interference, IE with the turret burried in the chuck and the sub plowing in behind them, i dont belive there are any safeties beyond the g28/30. So be librial with that 1% rapid override the first time.

EDIT:

A quick Google shows that g30's parameters are around param 1200, which i believe is correct. I found them originaly by just paging down

-Jacob

[MikieD]

You can do toolchanges at G30 reference points as well.

I do tool changes at G30 W0 U0 while the B axis is usually just left at G28 B0. On our 21LMS the G30 locations puts the tool changer around x0 z8 off the chuck, works great for just about any program.

You can change the G30 locations by enabling PWE and the locations are around parameter 1500 iirc (no book in fornt of me)

No ladder rewrite, service tech needed, you can edit this in 30sec standing at the machine.

Be forwarned however, from my experence, you can set the G30's to locations that will cause interference, IE with the turret burried in the chuck and the sub plowing in behind them, i dont belive there are any safeties beyond the g28/30. So be librial with that 1% rapid override the first time.

EDIT:

A quick Google shows that g30's parameters are around param 1200, which i believe is correct. I found them originaly by just paging down

-Jacob

Can I change the X location of the G30 south of home and still do a tool change? Right now I don't send the z anywhere and just send the x home. For my parts there is no need to move the z away so I eliminated that all together. That shaved around 10 seconds off the cycle time. If I can change the x's g30 would definately help some but the location would still be dependent on the tool that needs the most clearance and most of my tools don't need a third of that clearance for a safe tool change.

I still need to change the ladder because of the sub. G30 for B is the location needed to use the sub's part catcher. I have a couple simple parts coming up that if I have to send the b home for tool changes will double or triple my cycle time.

Have you tried to use multiple m codes per block on your machine?

[jvangelder]

You can change the G30's to whatever you want, you can make the g30 location's (there are 3) on the other side of the spindle if you wanted and watch as the machine tries like hell to get there. I belive you can even change the G28 location, not that you would want to, nice to have a zero location you can call.

I dont think you need a ladder mod for the sub either

You could do tool changes at G30 W0 U0 G28 B0

or G30 P3 W0 U0 B0

(g28 is first ref, g30 is second or g30 p2 is second ref, g30 p3 is third ref, g30 p4 is 4th ref)

Can you not do tool changes with the sub at g30 b0? i belive i can?

I dont know if i can run multi m's in a block, i havent tried.

Fwiw, our other fanuc machines that can use muilti m codes isnt really worth it. Usualy its just M3/4/5 with an m7/8/9 etc, not something that really saves time

-Jacob

[MikieD]

You can change the G30's to whatever you want, you can make the g30 location's (there are 3) on the other side of the spindle if you wanted and watch as the machine tries like hell to get there. I belive you can even change the G28 location, not that you would want to, nice to have a zero location you can call.

I dont think you need a ladder mod for the sub either

You could do tool changes at G30 W0 U0 G28 B0

or G30 P3 W0 U0 B0

(g28 is first ref, g30 is second or g30 p2 is second ref, g30 p3 is third ref, g30 p4 is 4th ref)

Can you not do tool changes with the sub at g30 b0? i belive i can?

I dont know if i can run multi m's in a block, i havent tried.

Fwiw, our other fanuc machines that can use muilti m codes isnt really worth it. Usualy its just M3/4/5 with an m7/8/9 etc, not something that really saves time

-Jacob

So I have 3 locations (p2, p3, p4) in G30 i can set for each x, y, b and still make tool changes? If so that will be a big help. It's the B it will help the most with. I current am only using G30 and don't use any p commands. If I'm following correctly g30 alone is by default g30 p2?

On the B... I can tool change at g30. I have to be at G30 B0 for the parts catcher to come up. If I send the b to the exact scond reference point without using G30 it will alarm out and say the sub ins't at the second reference point. I was thinking if I altered the g30 locations that the B would have to stay at 0 because of the catcher. If I have p3 and p4 though... I am curious about something else now. Since the catcher alarm specifically say "second reference point" does that mean I need to leave p2 at B0?

I don't see a lot of time savings using multiple m codes. In a few places of the program it would save me a second or two (I'm guessing around 5 to 6 total seconds off the part I have down to 2:15).

[MikieD]

Double post...

[jvangelder]

Yes, G30 is defaulted to G30 P2, p3 and p4 you have to call explicitly

http://www.star-circuit.com/article/...TER_MANUAL.PDF page 75 describes this

And you have 4 ref locations in total, i believe you can edit g28, i have just never tried.

When you get to them in the parameters page, it looks just like a work offset page, i believe you can even set the C axis in them.

I have a sub parts catcher, and also have to be at g30 for the parts catcher to come up. You can edit the g30 b locations and the catcher will still come up. We edit the location per job because of diff length parts. Ive never tried to call the parts catcher at g30 p2 b0 for example, im going to have to try this on Tuesday.

Sound like you have made quite a bit of headway without the sub and tool changes being in places you want, aprox 7min to under 3 is worth quite a bit of $ at the end of the day. Depending on tool changes you might get under the 2min mark.

-Jacob