On my Daewoo 230B with Fanuc 21IT control I am having a hard time getting tools set up. Tool number one is no problem. I am using G54 and touching off on the face of the stock to set the Z zero in the G54 work offset page. I am using the tool presetter to set the X offset in the geometry offset in G 01.
That works great. I then set tool 3 using the presetter in X and Z in G 03 offset. When I program to cut a 1.5 diameter shaft with tool three the tool goes to around .780 dia. in the X. The program calls for 1.5 but the axis readout says .780 and the tool will cut .780 dia. if I would let it. I can't understand why this is so far off. I have picked up the tools over and over again with the same exact results. Someone told me they never use the presetter because it is a pain and just measure the work piece and input that into the offset. What am I doing wrong. I bought this machine from a finance company used and didn't get any books. My Daewoo dealer got me one book on the machine but seems to have trouble getting the Fanuc books. I can't understand why that would be a problem but I'm thinking this may be my last Daewoo purchase if you can't even buy replacement manuals. :frown:
I really appreciate any help you folks could give.

Thanks
jim

I can only try to reason out the problem, as I do not have that controller.

Typically, the presetter has some parameters which describe the position of the presetter touch off point in the machine coordinate system (G53). I would attempt to adjust the X parameter of the touch off point, so that when Tool 1 (master) touches the sensor, the position of Tool 1 is diametrically correct in the G53 coordinate system.

In my mind, I do not want any X value in G54 other than X0, whereas Z can be whatever it needs to be.

If Tool 1 is set up in this manner, then its X offset will always be very near zero.

Now, when the other tools touch the presetter, they will most likely differ from T1. Whatever their difference is, should be the X offset amount for that tool.

In this manner, you won't be suffering from the complications of shifting the entire work coordinate system in X, which throws all the rest of the tools off.

I think where you are getting in a bind with your method is touching T1 off the part to set its offsets, particularly if T1 has some considerable amount entered in its X offset register. This causes you to be chasing two interdependant reference points.

Like Hu I also do not have that controller so I cannot give direct advice. One thing to look for is if there is a setting or parameter in the machine that controls whether the tool offset is referred to G54 or not. I have used a machine which had this type of option and if there was a value in the G54 offset table this was automatically subtracted from any tool offset entries.

In truth I agree with the person who advised you to ignore the presetter and just put things in manually. At least this way you know where you are and which way to change things to get it correct.

Touch the workpiece to set Z datum only. Then use the presetter to set the X values on all the tools. To check / set the presetter do the following.
1) Put a bit scrap material in the chuck.
2) Probe tool 1 with the presetter.
3) Call up tool 1 in M.D.I.
4) Take a test cut in M.D.I. i.e G00 X 20.00.
5) Measure workpiece. Should be 20mm.
6) Adjust parameter 5016 accordingly. (for O/D tools, 5015 for boring bars) the value is in microns.
7) Probe tool again.
8) Call Tool 1 in M.D.I. again
9) Take another test cut in M.D.I.
Repeat until the test cut size is correct.

Don't try to get less than 0.010 mm accuracy you will just go round in circles. Adjust that manually in the wear offset.

Hope this helps.
Alan B

My controller got the same manual so it probebly works the same. When I preset the tools and sets the zero point I usually does it like this:

Get the presetter arm down,
TOuch the sensor with all tools in X and z axis.
(all the values comes into Geometry offset and clears all wear offset values exept radies and tooltype)

After that I call a tool in MDI...

G0 T0202

And then I position the tool at a known point. (Ex were I want the zero point)
And then in the work offset screen, position at G54 and then Z0 messure

And that is All. Just have G53 work offset put at zero.

There ar really not any MAster tool used with this option and it a smooth and easy way to messure tools and zero points.

This is really great guys. At least now I have a couple of methods to try.

Thanks so much.

Jim

Alan-B is right on, Your Pre-setter needs to be calibrated. It has probobly never been used. Also in the parameter config there are settins for Dia and Rad you need to make sure they are all corerct. Now I am going by my 16 and 18I's but the 21 should be close. I have a 21I manual and I am still looking for the info on calibrating the pre-setter when I find it I will send it to you.

Bluesman

This is what Alan is talking about, And I have the 18 and 21I manuals and they are the same


Bluesman

Hey Jim see if you can download this it is a big file, I have almost every Fanuc manual from 16 to 21I on disk now the manual I have here says it is for 16 and 18 I (b) but the condensed version I have is for 16 18 and 21I (b) style so they are the same. The book here is from 2001 and I do not think the 21I was here until 2002. Anyway if you are having trouble getting this from DEAWACK then it may help. And yes DEAWOO blows the service is for crap. unfortinately we have a bout 15 of them and it is to late to by what I wanted. Anyway I hope you can download this

Bluseman

Try again

Nope it is to big 500mg max Its about 2500 send me a private mesage with your e-mail and I will e-mail you all I got


Bluesman

I found out what the problem was. It had nothing to do with the presetter.

G54 is not a model command on the machine. You have to type in a G54 in every line that has a tool change. Oh well, I bet I never forget that little detail after screwing with it for two days.

Thanks again for all the help
Jim