[Rob_N]

Hello, I'm trying to decipher this type 88 controller on a 1980's Fadal 4020...

I am able to DNC programs to it via NC assist and currently I've been cheating part of my setups. I'm using G54 for my offset because that's what I'm used to on Fanuc controls I use at another job shop. and my post works as well.

1) After a board recently went out and had to be replaced I am getting some additional movements at the mill that are not in my program. They seem to be inserted at the machine when I start a program. The machine moves to X0Y0Z0 before starting the DNC sent program. I really need to get rid of this as sometimes I like the bottom of the workpiece to be Z0.

2) I set my X & Y by getting the machine to the center of my workpiece then typing SETX then SETY... Now for the cheat... I do not know how to set Z offsets and use the tool changer so I just touch my cutters off of a known gauge block on the top of my workpiece then SETZ, then I manually move the Z the size of the gauge block and SETZ again. All of my tools are T0, and H0 in my G43 line.

I've been getting by with this for awhile, but since things are slowing down I'd like to sort it out and make life easier.

[DareBee]

The issue isn't the control. you need to leave your G53 Z at 0.
When you do a set Z this changes that.
Your ATC will crash with the Z home changed.
If you are calling for (and using) G54 make sure you set the X,Y and Z zeros within the G54 offset on the offset tables.
Try inputting your offsets by typing DF in the command line and using option 4 (I think).
I believe you will need to start using tool length offsets if you want to do multi-tool programs as well.

Start and end headers are important - here is a sample for you to look at, as far as start/end code goes.

%
N1 O9 (ENREW)
N2 G0 G40 G49 G80 G90 G17
N3 (SCREW ROUGHING 1 - .5IN 4FL BALLMILL)
N4 T8 M6
N5 G0 G90 G58 X-11.87 Y0 A0
N6 S1240 M3 M8
N7 Z8.145 H8

N408 G80
N409 M5 M9
N410 G0 G90 H0 Z0
N411 E0 X0 Y9.9 A0
N412 M30
%

[Rob_N]

So by typing SETZ I am changing the Z home?

I guess that's why the ATC crashes into the head...

I do not know what to expect on the Fadal. I assume its like the Fanuc I have at my day job.

@ Z home I make sure the Z number is Zero, I then hand wheel down and touch off a 1" gauge block. I goto the tool offset table, find my tool # then press INPUT. It fills in the field with the number. I then type 1. and press INPUT+
This allows me to use the G43 with H#, with or without using the ATC, which is what I'd like to do on the Fadal as well

What is the correct way to set the Z height of a workpiece and use tool offsets.

[DareBee]

IDK if you are using space bar menus or not?
So we will do command line style.
This is off the top of my head (you may need to read between the lines a bit )

Set tool offset =

Type DT <>
Pick option 4
Enter starting and ending tool numbers to set at prompts.
Pick "set length" at next screen (option 1 or 2?)
enter height block size at prompt.
Pick option "jog to locate" (#2 I believe).
Jog and contact your block press enter<> when done.
press "start" when it asks to press start.
- that tool is set and the machine will be at the TC location with the next tool loaded ready to set it (assuming you chose more than 1 tool to set the length).

Fixture offset =

type DF <>
Pick option 3 (utilities)
pick option 1 (set offset number)
choose your offset # (you said you wanted G54 that would be offset #1)
pick option "locate fixture"
input edge finder dia
pick option 2 "jog to locate"
start spindle and edge find an edge.
press manual when done
select option 3 "store location"
press X or Y depending on which axis you have just edge found
input + or - to set edge finder offset.
repeat for other axis
your Z axis offset will likely have to be calculated and typed in.
I ASSUME you have zereod your tools on the table (judging by your prior posts) so your Z axis offset will be a + number = to the distance above the tool zero that your part program zero is.
EXAMPLE
If my 0 in my cam program is the top face of my stock AND my stock is in my vise on parallels I have to measure (or KNOW) the height of the top faceof my stock to the table.
In my FO (fixture offset table) I enter THAT distance as a + (because it is above my tool 0 plane) into the Z spot of the corresponding fixture offset (in this case offset #1 because you are using G54).


The basics of how this system uses the offsets is the same as a FANUC program just a few different methods of input into the control.
There are a dozen ways to input these offsets, this is just 1.

[DareBee]

Please be aware that I have made the mistake of assuming you are operating the FADAL in format 2.
If you are NOT please disregard my posts and consult with somebody who uses Format 1.
I have never done so.

[Rob_N]

I haven't been over to the shop this week, I forget what format # it's in.

That's the rough part, I only use this mill a couple of times a month.

Thank you for the info though, I should stop by their sometime this week as I need to get paid, LOL

[Bwana Don]

I went around and around with my Fadal and the offsets. Here is a few things I did to make my life easier. Bear in mind there is always more than one way to get the job done.

My Machine is a 1998 3016Ht with the 88Hs controller.

Overview
Machine Home (Machine Coordinate Position);
Also known as G53 X0Y0Z0 (Z0 is the tool change height)

HO Automatic return to zero of the "Tooling Coordinate System". In my machine TCS and MCS are both set the same. This is also the Cold Start Position. Which is the middle of the table (tabs) for XY.

What I did.
Use Format 2
Move your machine to the middle of the tabs, XYZ. Type in setcs, hit enter.
Your machine moves to the MCS.
Type in SetX, hit enter
Type in sety, hit enter.

What Just Happened.
The CS, TCS and MCS are now all the same. (XY only, Z is set for the tool changer position)
Check by typing, in MDI mode; G53X0Y0, hit enter and machine moves to middle of x and y.

Datum Setting;
E0, this is TCS, MCS. in MDI mode type; G0G90E0X0Y0, hit enter. The machine should move to the middle of X and Y

E1-E36; These are your fixture offsets. Access them by typing in DF.

Set your datums in relation to the E0 datum (MCS,TCS) Your screen needs to verify your in E0 datum PRIOR to setting another datum.
You can set multiple datums, leave a vise at one end and NOT move it. Call it E10, whenever you use it, use E10. No datum setting (provided you moved nothing).

Ending a Program.
This has been a tricky area for me. There may be better ways to do this but, it works for me. I'm open for suggestions on this.

Here's what I do.
N354 G0Z4.M5M9 (spindle up off the work piece with a Z move, spindle/coolant off)
N355 G53Z0 (G53 is the MCS, Z0 should be tool change height)
N356 G53X-5.Y7.5Z0 (another G53 with X move and Y move to bring the table to the front of machine for loading)
N357 M2 (end of program)
% (rewind program)

I think that's it. Did I make any glaring mistakes?
Keep in mind this is one guy's way to run the machine, you do your own thing.
I had a Professor in Industrial Management classes that use to say; "There are three ways to do things. the right way, the wrong way, and your shop's way".

Good Luck. I hope this helps.

[Neal]

So far so good!

Neal

[Bwana Don]

So far so good!

Neal

Thank you Neal. I learned pretty much on my own. Cussing, reading, trying things out. Over ten years I have come to know this Fadal pretty good.

Oh yea, Macomb Community College helped. The three or four CNC classes I took gave me a good foundation.