Mori Seki SL1 NC lathe programming

The control may only be able to handle one M code in a block/

John

The G98 may not be used on that machine.

John

Thanks John, I discovered that only one M code is allowed, that helped. I think I may have some other problems with parameters. I will post another question on that problem. I am still having the error message but the parameters are wrong.

thanks Keith

Are you sending this program to the machine?

It could be that your parity, or other comm setting is wrong.

Try sending from the machine to the computer.

My machine does not have the rs232 port to send out from machine to punch or BTR but when I look manually at the content of the addresses the program seems to be there correctly downloaded. I think I just have to get more familiar with the conventions required.

I plan to do a one block at a time download to see where the problems occur.

I am confused by the g50 command. When the machine is zeroed the x and z coordinates are 0 and 0. Why do I need the g50.? Is is possible to change the absolute coordinates of the zero position for x and z? How does one know what values to enter?

Thanks Keith

I'm a little confused. You said you have a BTR, which to me means a board that emulates a tape reader/punch so you can send info to and from a computer. Is that correct?

It is possible that you are putting in some codes that your machine doesn't like, such as the 2 M codes in one line. If I am correct in what you are trying to do, it is also possible that you're getting some noise from your communication line. If you're sending code from a computer, make sure that you are using a text only word processor. Sometimes, if you're not, the software may send a formatting or other hidden character that your machine does not understand, and can't display. Or, you could be overflowing the buffer on your older machine and dropping characters (probably not on that short of a program).

Keith,

G50 is your tool offset geometry and you need it for each tool. Normaly X is to centerline of spindle and Z is usually to the end of your completed part.

Zero Return the machine Origin X and Z axis if not 0 in each counter Index to tool Start Spindle

Face off your part or touch the front. Z axis reading + or - whatever the raw material condition is and this is your G50 Z input.

Turn the OD X axis reading + the OD diameter and the answer is your G50 X input.

Now some machines the Z could be Z- or + so you need to work that out and X is the same way.

In this example I am assuming Z zero is the finish face (length) and X is Zero is Spindle Centerline.

Tool #1

Z axis at home counter is 0. Face off part and the counter reading is Z9.850, you check the part and you have .025 material left to face off. Z = 9.850+.025 = 9.875

X axis at home counter is 0. Turn the OD and the counter reading X5.908 mic the OD and the part is 1.507. X= 5.908

• 1.507= 7.415

In this example G50 X7.415 Z9.875

Once your tools are set and you don't change the tool you never need to change the X value. For Z you only need check one tool then make the same adjustment to all the others (this is equivalent to a work shift).

For drills indicate the center of tool holder and that is your X value and that will never change unless something changes on the machine.

For my example it assumes you are programming X+ values and Z- values.

Tom

snipped-for-privacy@cox.net wrote:

I see the logic and this is described in the manual but I did not realize I had to enter a g50 for each tool. I may have been confused between g50 and tool offset. It seems like with tool offset feature I could enter x and z tool offset value obtained as you have described for each tool. Then, I would not have to issue g50 for each tool?

Thanks, Keith

I would start with a very simple program to check the data link...Turn the spindle on, turn it off end of program. That machine may not have a lot of stuff like newer machines have... like a G50.

M03 S200 M05 M30

Then make a prgram with a simple X move and Z move. Use only G00 codes and G01 codes with a feedrate.

One thing at a time until you find what it takes. Or get a programming book for the control with all the info in it.

John

============= What are you using for an editor? In many cases a general purpose editor program inserts non-printing control characters with the text. Try using a cnc specific editor. You can also download one of the old DOS sector patcher programs to examine the file character by character. This can be helpful if you can down-up load programs from the machine to the computer but not programs you write on the computer to the machine. Typically the manuals never mention this, but the programs written on the machine and downloaded to the computer will contain non-printing control characters.

Just a though.

Unka George (George McDuffee)

There is something to be said for government by a great aristocracy which has furnished leaders to the nation in peace and war for generations; even a democrat like myself must admit this. But there is absolutely nothing to be said for government by a plutocracy, for government by men very powerful in certain lines and gifted with the "money touch," but with ideals which in their essence are merely those of so many glorified pawnbrokers.

Theodore Roosevelt (1858-1919), U.S. Republican (later Progressive) politician, president. Letter, 15 Nov. 1913.

Sounds like a good suggestion. I just discovered that I have a Yasnac

2000B not G but Yaskawa says to use the G manual. It does have a G50 supposedly. I'll see if it works line by line as you suggest.

Keith

Thanks, good suggestion!

Keith

Keith,

The terminology has evolved so with the older manuals it can be a little misleading.

G50 is your Tool Offset, and yes you need it for every tool. "Tool Offset" referred to in your manual is really the Tool Wear Offset.

(Be careful that G50 is calculated at tool change position and I have assumed in my example that G28 X0.0 Z0.0 is your tool change position. I did not want to confuse you with too much information but your format is important. If you use a secondary tool change position such as G30 then that is where you zero out the counter and figure your offsets.)

I do not know the exact G codes for your machine but for safety and easy restarting I format something like this on an older lathe. For yours it will be different since you can't have two G codes on the same line.

"Start of tool"

N1 G00 G20 G40 G80 G97 G99 (safety) G28 U0.0 W0.0 T0000 / M08 (tool change position) G50 X? Z? (tool # 1 geometry offset) G97 S2000 M03 T0100 (Start Spindle, Tool Change) G00 X ? Z ? T0101 (rapid approach part with tool wear offset)

General machining movements

"End of Tool"

G00 X (clear part) Z (clear part) G28 U0.0 W0.0 T0000 M09 (tool change M01

Tom

snipped-for-privacy@cox.net wrote:

Keith,

John is absolutely right about doing a few little things at a time. Old machines like yours can have some surprises, what we take for granted now is not safe to do with your machine.

Tom

john wrote:

Thanks Guys,

I am still confused but once I can get the machine running and experiment with the thintg I think I will understand it. I was confused by the offsets and now realize how they would be used for wear compensation. Unfortunately I am trying to be a machinist by the trial and error method and although I have command of my cnc mill, I have no experience with a cnc mill. I have command of my manual lathe so am familiar with that. I really do appreciate your help and know it takes time to formulate the responses and check the posts!

Thanks again, Keith

Thanks Guys,

I am still confused but once I can get the machine running and experiment with the thing, I think I will understand it. I was confused by the offsets and now realize how they would be used for wear compensation. Unfortunately I am trying to be a machinist by the trial and error method and although I have command of my cnc mill, I have no experience with a cnc lathe. I have command of my manual lathe so am familiar with that.

I really do appreciate all your help and know it takes time to formulate the responses and check the posts!

Thanks again, Keith

Tom, Dan, Cliff, and everyone else

Thanks for this detailed discussion. I did not expect such a naive question to generate the discussion it did. It appears to me that what Tom described is exactly what is detailed in the Yasnac manual for setting the G50 x and z. It does not seem to matter what the configuration of the tool tip is since we are only interested in the orthogonal planes of movement by x and z. Consideration of tool tip compensation for curves seems to be irrelevant to my question.

When I posed the question, I was under the impression that my lathe was so old that it did not have G50. I was trying to understand what it did so I could somehow work around it. At that point, every time I tried to work with G50 the machine responded with an invalid character error. I finally stumbled on the fact that it does not use decimal points! Too bad the manual fails to mention that important point. Now I am able to begin to work with machine and can actually get the axes to move to my programming advances. You can understand how confused I was when nothing seemed to work and I figured the manual was for a more modern machine. Hopefully the compensation feature described in the manual will work on my lathe so it will all be done automatically for me when I get to that point in my learning.

Again, thanks to everyone for their input!

Keith

Keith,

Your original posting had to do with determining G50 values and I did not realize you were having trouble with the units or data input format. This will probably happen a lot for you because of the age of the machine. Keep a list going as you figure them out.

Tom

snipped-for-privacy@cox.net wrote:

Tom, Unfortunately I did not know that I was having trouble and just thought the machine was not recognizing the G50 command. I am using Bob Cad/Cam and they have a post for the Yasnac 2000B. Hopefully that post is compatible and will speed me along.

Thanks again, Keith