What's new
What's new

Deckel FP3NC - debug connection to PC

ivang

Plastic
Joined
Oct 4, 2021
Hello, guys,

I'm glad to be part of this really nice forum!

I have one really silly question about Deckel FP3NC - is there a way to debug communication between Deckel FP3NC and PC via RS232?

A colleague of mine used to use and maintain the machine.Unfortunately he passed away due to Covid complications... Hope he is on a better place now! All the knowledge about the machine gone with him.
I'm trying to bring-up the machine now, but I'm an electrical engineer and I don't have any practical experience with CNC. I found the User's manual for Deckel Dialog 4, and based on it I was able to start the machine, move on X,Y,Z in modes 4,5,6, so I think the machine is working.
Now I'm trying to load some programs via RS-232. I have the cable my colleague used, checked it - it's OK, all wires are properly connected and soldered well, no faulty wiring or short circuits.
Regarding User's guide, mode 14 has to be used to transfer files to CNC. I did the following:
- selected "Mode 14" from knob;
- with <> went to interface selection and selected RS-232;
- in RS-232 menu selected 9600/8/n/1;
- went back to main menu;
- selected "In" mode;
- selected program 100 and pressed "Transfer" button;

And everything stops here. I have NCPlot v2.34 installed on PC. PC is equipped with hardware RS-232, not USB-to-Serial. COM port is working, check it with loopback cable. When I try to transfer some .nc file, NCPlot says "Transfer completed", but nothing happens on CNC. COM port setting are the same as CNC.

Could you please advise me how to proceed.
 
Dialog 4 is very particular as the exact format it will accept for file transfers....

First some hardware notes....
I would not use 9600 baud...that is too fast for that aging interface, you will have fewer errors using 4800.....
Also i never use any parity....My machine runs 4800,8,1...
You must have computer and control set the same...this is a pretty dumb interface....(old tech)

The control must be set to receive in mode 14 ....Set to mode 14....with cable connected.
Press the "Acknowledge" key (the white diamond with the "J" on the left side) You should get some white highlighted boxes on the screen ...
At the very top the "IN" should be highlighted.
There should be highlighted boxes at the top : %, %#, D, T, P

On the left below the above line should be highlighted something like: > then a % and a number.....(this is the currently active program in memory if present)

Finally at the lower part of the screen should appear a rectangular box with: % ?.

Then you need to press the transfer key...(the green diamond with the >...)
The screen will change and show a highlighted rectangle about 1/3 down on the left , showing: > % ?

If you get all this the control is ready to receive...but the flow needs to be initiated form your PC.....This transfer really runs without any flow control....

Once the transfer is started, the scree will change and you should see the number you selected for your program (must not be the same as any programs already in memory (check in mode 13 before assigning a program number)
The program number (defined by the % sign) will appear on the left side of the screen and you should also see the block numbers counting as the file transfers....

If it tries to send but you see ???? and no numbers changing as the file loads, then your format (header) on the file is not correct.

If you get this far, might have a look here:
https://www.practicalmachinist.com/...config-149130/?highlight=Dialog+file+transfer
for details on the file format...Be aware that in my post showing the header and footer (#12) i wrote them backwards....the footer appears above the header and of course that is not correct...Sorry for the confusion.
Cheers Ross
 
Dear Ross,

Thank you so much for your detailed answer!
I followed your instructions and the code was transferred without errors.
I've set the baud rate to 1200 bps to be able to see the blocks counter increasing during transfer. As you mentioned Dialog 4 is really sensitive to file format, header and footer content. There were several Errors during transfer.

After transfer I was able to see the program listed in mode 13 with memory size, comment.
Regarding manual, in mode 13 program can be displayed:
- select program with up/down arrows
- press %0 and "Transfer" key
The program is opened, but there is no code inside.
If I select the program and press "Acknowledge", the program is loaded in memory and I can read it block by block in mode 11.

I will try to run the code now, it's just simple movement on X,Y.

Regards, Ivan
 
Hi again,

Machine is up and running! I was able to transfer file and execute it.
I used following header and footer:
For inch files:
%
($%4/000000)
N1 X-.6549 Y+0.0112

N9999 L0 %4

?
0000
$%4

For metric files:
%
(&%4/000000)
N1 X-.6549 Y+0.0112


N9999 L0 %4

?
0000
&%4

Regards,
Ivan
 
Ivan:
Welcome to the forum.
FP3NC with a Dialog 4 control is a nice bit of kit. Not the fastest control but quite capable!

Very easy and direct operator interface, think you will like it.

Quick note:
It is not necessary to transfer the tool data with your file transfer.
I never do that as i set the cutter length offsets using the machine itself to compare all the tools in a program and since i will be entering (mode 10) the offsets after making my measurements there really
is no reason to fuss with entering them in the header....

Note might be unnecessary ,just looked at your example above and seems you are not transferring the tool data...so forget the above info....

Some info you might like...There are two versions of the Dialog 4 control (a hardware change).
If you use the operators station to enter program data (MDI)
Go to mode 13.
Hit %and a number (not already in the program list) then hit the transfer key
The number you selected will appear in the program list....

Should be highlighted, Hit the acknowledge key to make the program active....
Then go to mode 11 and you can start entering program moves directly.

When you go to mode 11 there will be a highlighted rectangle at the bottom of the screen: N 1

Hit the transfer key and "N 1" will appear at the top of the screen...
You may now enter code directly....
Cycles like drilling and circular interpolation will prompt you for each required value to make the requested code work.....

If you enter "G 3" for example to cut a circle, you will be prompted for the Feed rate,(F)
The end position of the cut in "X:
The end position of the cut in "Y" (or Z) depending on weather you are using the vertical or horizontal spindle...
Then you will be prompted to define the center of rotation of the circle or arc in the "X" axis looking to the center point from where the tool starts the circular move. (this value will be incremental) The program assigns "I"
to this value.
Then you will be prompted for the "J" value (K if working horizontal) This is looking to the center from the start from the starting tool location along the "Y" axis....

Ok so now here is the point.
You will either be asked to enter a "Z" value after all the above has been filled in..or there will not be a "Z" value to be supplied....
If the control asks for a "Z" component to the circular move then your machine is capable of doing "Helical Interpolation" (think threads)

That is a good thing! If you are doing a plain 2-D circle and don't want or need a depth change you can just transfer key and the "Z" (or "Y" if horizontal) will just disappear....

If your control does not ask about a depth component then your D-4 is the early version and can't do real helical interpolation....


Everyone has their own technique to program.....
Here is my technique:
I always start every program at the same place....
First block i position the tool at a tool change height off the part...my usual is 4.0"
I always position the spindle at "X" 0.0000" and "Y" 0.0000

Second block i define the tool and the plane that is used for setting length comp....



So for a vertical spindle program it looks like this:

N1 G0 X0.0000 Y0.0000 Z 4.0000
N2 G17 T1
N3................


For a horizontal program:

N1 G0 X 0.0000 Y 4.0000 Z 0.0000
N2 G18 T1
N3..........................

The G0 is a rapid move to position the tool at the called location..no spindle rotation required.
The G17 defines the cutter comp to be controlled for length in the "Z" axis (Vertical operation)
The G18 defines cutter length comp to be controlled in the "Y" axis (Horizontal)

The Deckel manual (hope you have one) is pretty good with examples of the programming...
Hope the above helps you get started...The board here can help with any questions .

Cheers Ross
 
I do a lot like Ross, except my first move is just a retraction, so either G0 Z4 for vertical or G0 Y4 for horizontal. That way there's no sideways move to risk crashing into something. I do the retraction, call the tool, turn on the spindle with S+nnnn, make the sideways move far from the work, G0 X0 Y0 for example, and then approach the work, as in G0 Z0.06. I then do a further Z move to my safety plane, like Z0.05 F10. If you don't make at least one move with a feed rate before jumping into a compensated contour, (G41), the program will barf even though you provide a feed rate within the G41.

The machine feeds much more smoothly using G41 contour compensation as opposed to feeding it simple moves (even arc moves) from CAM while letting the CAM do the compensation. It is easy to choke the control with CAM-fed programs, which leads to lots of feed dwells, marked work, and dull tools. I find it hard to choke it with finger-CAMed G41 moves. Dialog forced me to get really good with finger-CAM.
 
Hello, guys,

Thank you very, very much for the posts! I've spend previous week with the Dialog4 operators manual, there is a lot of information about language and machine capabilities at all. I found a folder with a lot of old programs, created by my colleague. I will try to execute some of them.

One question here - most of the files contains some meaningful information in the header and footer instead of zeros. As far as understood this information is size in bytes in header and checksum in footer. If I do modifications of program body, header and footer must be reset to zeros before transfer, right?

Regards,
Ivan
 
Yes, reset the header and footer hexadecimal numbers to zeros. I don't remember what happens if you forget to do that. At a minimum, the code won't load and at worst, you'll have to reset the control by pulling the K10 jumper inside the console.
 








 
Back
Top