Dialog 4 Contour Pocketing error code 88

Hello everyone,

I am currently trying to understand the G79 contour pocketing cycle of my Deckel Fp2NC(2801) with Dialog 4
When programming a Pocket using the G79 contour pocketing command, I get the Error Code 88.
The control always mentions the error with the sentence which calls G79; e.g. Sentence N3 calls G79 I get the Error N3 88.

My documentation says error code 88 is a programming mistake, too small milling row pitch or the control is not capable of doing the G79 cycle.

I tried some of the sample G79 Programms from the Deckel Dialog 4 programming handbook with different cutter diameters, but even then error 88 strikes.

Is there a possibility to display the available G- and M- Codes on the operator control´s display?
How can be missing cycles be unlocked? Are the unlocked cycles independent from the Dialog 4 software version?
My Deckel has this software versions installed:


Can someone of you help me with my issues and provide me with some help?

Kind regards,

Markus

3.07 is a late version IIRC, so nothing should be disabled. Can you share your code and your tool table? I doubt any relevant cycles are locked. Rather, the pocket is not big enough for the size cutter or some issue like that.

I see that G79 is for contour pockets with islands. I have never used G79, so maybe it is disabled after all. I use CAM for oddball pockets, or program from simpler G41 moves while taking advantage of the ability to move in Z during a G41 contour compensation move.

Not an ace regarding the software versions....But yours seems to be a bit strange to me....
That is a very late package for a dialog4...3.07 i believe is the latest version...However your NPP and NRP software is pretty early....For a 3.07 think the other two should be around 2.33 and 2.32...

When you program or call a circle or arc...(G02/G03) does your control prompt for a depth component ? Can you program a helical move in other words....

As to seeing the "G" code for the cycle...Don't think it works like that.....The cycles are integrated i believe no individual moves...its all run as one overriding cycle...hard programmed, and hence you can't view individual parts
as in fact there really aren't any.

Cheers Ross

In my experience the error diagnostics are pretty good, though occasionally the control will show an error code (like "88") because there is a programming fault, but not necessarily the exact fault listed in the documentation. Post the exact code you are running and we can help diagnose it.

Thanks a lot for helping me out with my problem :-)

Perhaps CAM is the way to go for these odd contour pockets, but I like the idea to program such a pocket from a quick and dirty hand-drawn sketch.
Of course it is possible to build a complex pocket from square and round ones....

My understanding for G79 to work is:
With the actual G79 promt you tell the control how to clear the pocket.
Then you define with G41/G42 your outer geometry of the pocket.
After G40 for the outer contour you can add up to 7 islands which are programmed similarly , too.
You close the pocket definition with M79/M78.

There are actually even error codes for programming mistakes inside the contour pocketing cycle; e.g. Error 84...

This is one of the programs I tried to run. It is the outer contour of the example on page 6-130 in the (german) programming handbook.
I did not program any islands for the ease of programming and wanted obviously just cut some air.

%15
N1 G0 Z100
N2 T1 G17
N3 G79 Y5 X1 F100 Z2
N4 G0 Z2 S+2500 M70
N5 G1 Z-5 F100 M70
N6 G41 G47 A2 X5 Y25 G0 G60 M61
N7 G1 Y5
N8 G7 R4.5
N9 G1 X78
N10 G7 R15
N11 G1 X97 Y75
N12 G7 R8
N13 G1 X5 Y65
N14 G7 R4.5
N15 G1 Y25
N16 G40 G47 A2
N17 M79
N18 T0
N19 G0 Z100 M30

For T1 I tried:
T1 R3 L0
T1 R3.5 L0
T1 R4 L0

The error code that gets displayed is "N3 88"

My control does call for a "Z" component when programming a circle move. The thread milling cycle does work, too.
Package 3.07 is mentioned on the dialog5.com site as the latest software version, too

Well... it does not surprise me, that some software version of the individual cards are somewhat mixed....
The previous owner seemed to have upgraded the mill in the past...
It was build in 1980 and as you can see in the screen shot in my first post, there are the "90s" cards installed in the PLC. In the electrical cabinet there are (text)remnants left, which mention the older "PC1" cards.
The mill (it is a Fp2NC) came with the big (7 T-slot) FP3NC universal (rotating, swiveling and tilting) table with digital readout, but the NZP59 Card + EXE for the C-Axis are missing in the operator's console.
There is no C Servo Amp in the cabinet, too.

Cheers,

Markus

What happens if you change N2 to G17 T1 instead of T1 G17?

Ran this on both my Dialog 4 machines with 2.33 software-won't work as written.
Will run correctly if you eliminate the M70 command from Block N4.
Also, G1 is a modal command and you don't have to enter it on every block, it's not needed anywhere in this program.

That makes a whole lot of sense. I only use M70 with out-of-plane moves and to set feed rates, and without G0.

Colt45 said:

Ran this on both my Dialog 4 machines with 2.33 software-won't work as written.
Will run correctly if you eliminate the M70 command from Block N4.
Also, G1 is a modal command and you don't have to enter it on every block, it's not needed anywhere in this program.

Click to expand...

I just tried your suggestions on my machine.
But I still get error N3 88.

For Block 4 you just wrote "N4 G0 Z2 S+2500"?
What error do you get if you program N4 with the M70 command?

rklopp said:

What happens if you change N2 to G17 T1 instead of T1 G17?

Click to expand...

Don't think he can actually write the program in the control as he shows here...the compiler of the Dialog will set the order of the commands no matter which way he enters the commands...
Think it will always appear in the control as "G17 T1" no matter which way its entered (when doing MDI of course...going with code fed from a computer (RS232) think the order will be entered as the computer sends it.

Cheers Ross

Neeroy said:

I just tried your suggestions on my machine.
But I still get error N3 88.

For Block 4 you just wrote "N4 G0 Z2 S+2500"?
What error do you get if you program N4 with the M70 command?

Click to expand...

I got it to run this morning on both machines, by only changing block N3 as follows:

N3 G79 X1 Y5 F100 Z2


The example in the book is formatted incorrectly for this block and also, as mentioned, for the tool call- should be "G17 T1".

Sometimes the Dialog control will show an error code and the problem is not the exact problem and it might be in a subsequent block to the one listed.

Dialog is very particular about syntax and format. When in doubt, it's good practice and eliminates a lot of minor mistakes if you hand code on the console.

You got it to run, but does it make the correct pocket as per the manual? I wonder whether swapping Y and X has meaningful consequences for the width and step-over, for example.

Yes, makes the correct pocket.
I have the same example in my manual, looks exactly like the drawing there.

Steve:
Guessing you are transferring the code form a computer,yes?

The syntax of the manual might not be correct, but if you are entering the program via MDI at the console you can't enter it incorrectly, the dialog will put the characters in the proper order automatically.

Bit interesting this...i entered the program (MDI) as written, syntax is correct....won't run for me either...I get the "88" error at line 3. Never used this cycle before i don't believe...Tried some different tweeks, no go.


Cheers Ross

I have tried now for Block N2 "G17 T1" and "T1 G17" as well as for Block
N3 "G79 X1 Y5 F100 Z2"
I get "N3 88" every time.


Changing the order of X and Y in the G79 promt will alter how the pocket will be cleared.

Attached you can find the (german) description of the G79 call.

Translated to english:
G79: Call for contour pocketing
Control will ask for
X(Y)(Z)*: Cutting width and direction for clearing operation
y(X)(Z) : Starting point and axis direction during clearing operation
F : Feedrate
Z : Withdrawal distance in Z
D : Tool length compensation number (if not needed: Enter-Key)
Z : Distance from milling ground

*) When milling with the horizontal spindle: Y and Z are inverted

I tried to contact Mr. Singer now, but haven't received a answer from him, yet.

Entered direct on the console, on both machines.
Was able to enter it exactly how he has listed by changing the X to Y at the prompt, and neither machine will run that code with "Y" first.
They WILL run the program and cycle if the prompt order is retained, with X first..

It is possible in this cycle and some others (G72*1 comes to mind) to change the X or Y (or Z depending on which spindle is used) value when prompted. The control will then make the next prompts in the new axis, and the later prompts (for the other axis) in the tangent axis. The manual recommends changing the prompt so that the "long" axis of the pocket dimension is first, because the control will more efficiently clear the pocket that way. Does'nt seem to work in this case, though.
Changing the way the pocket is cleared does not change the dimensions of the pocket.

Some additional information on this and a question....

Loaded the program into my second FP4NC this morning...This is a Dialog 4 machine with software package at 2.19.

Program ran without flaw as the OP had written it...
Tried changing the position of the "X" and "Y" on line #3 ...no change , program runs fine either way only difference is the direction of the clearing cuts...

Looked again at the program loaded on my software package 3.07 machine (FP4NC) ...will not run. Same program, same syntax...everything!
The later software machine gets the continual error:"88" on line 3....

So here is the question. Neeroy, Have you actually opened up the large electrical cabinet and verified that your machine actually has a PC2 fitted....
Now i know that the software list you provided via screen shot says yours is a PC2.....BUT my software 3.07 machine screen says it has NPP 90 fitted (PC2) when in fact its really a PC1 .....

Looking at your screen shot, your NPP SYS is listed exactly the same as my PC1 machine....Might be the problem.

Cheers Ross

I just come from the shop looking into my electrical cabinet...
There is indeed just a "PC1" installed.

Perhaps the older machines got new Eproms for the PC1 during on of these Software upgrades.
Does someone of you know any details how these upgrades were carried out?

I thought the PLC in the cabinet just controls the machine I/O like gear change, lubrication etc, while the control in the operator's console calculates and controls the actual moves and tells the PLC what to do?
Isn't the hardware for the positioning loop located in the operator's console aswell?
But all the Information summarized, I found about the PC1 and PC2 PLC is just like: " Well yeah... there is the older PC1 and the newer PC2... difference is negligible".

By the way I still haven't heard anything from Mr. Singer. He was busy yesterday when I tried to call and his employee suggested to write an E-Mail.

I share your impressions relative to the "PC" , however it is not lost on me that the two machines in this discussion that won't do the pocketing routine are both fitted with a PC1.
Perhaps its just coincidence...but i do not think so.
Further, The later PC seems to have more "options" that the user can select via DIP switches.

I have no documentation for the PC1, but the orange book does define the functions of the switches on the PC2 boards.....so there does seem to be differences between the two.

As to upgrades....You have to purchase a machine set of E-Proms.and physically change the chips....there is no downloading...Software is burned into the chips so an upgrade requires
changing physical components

Components get swapped (boards) when trouble shooting ...can get combinations that don't work well together i think. Other issues exist as well. Some versions have rounding errors for the
position/ math calculations.
Some versions also have issues with loosing a few tenths (.000X) when entering a value, or making a called program move if the direction or entered value is negative. This seems to only to be a thing when workign
in inches......

Cheers Ross

The G79 Contour pocketing cycle now works on my machine :-D

After some phone calls with FPS and another Deckel service technician I found the solution to fix the dreaded Error 88...

First some Information and a assumtion:
PC1 and PC2 just control machine functions like said before. PC2 was introduced to provide more I/O functionality for the tool changer mills.
Additional cycles for the Dialog 4 control can be unlocked using the DIP switches on the "NPPx0" card.
NPP90 offers a finer grade of "unlocking", e.g. there are 2 sperate switches for Graphic and the contour pocket wile NPP80 has just one for both.

Now my assumption is, that software package 3.07 came with Graphic included and you had to pay for G79 to work.
because Graphic was active on my Mill but the DIP switch for Graphic + contour pocketing on my NPP80 was off.
After changing it to on everything works fine.

If you want to know which switch to flip, please PM me. ( I just don't want to get anyone offended, when writing this information on a forum board open to the public.)

Kind regards,

Markus