What's new
What's new

How to/ where to find file transfer deckel

Trabantman

Plastic
Joined
Jun 21, 2012
Location
Netherlands
Hi Guys,

Always reading a lot over here and getting most of the info i want.

But finaly i have got the postprocessor for my deckel Fp5NC.
Whit the 3.07 software and the NEP 52 and NPP 55 like i read here multiple times.

So think i`m on the right way but i don`t have the manual how the 14 and 15 controls exactly work.
So this way i can find out if everything work out fine ?

Got a test program ready but not sure how to select it to the deckel to get the info in.
I can put transfer file but there isn`t seem to happend anything, maybe i got the name wrong.
In the post at the first line stands %123 is that then the number i need to fill in on the 15 when selected IN ?

Hope you can help me out, or have a manual were i can find everything to work it out.

Thanks Remco
 
I presume from the mention of 3.07 software, this is Dialog 4... not 11, yes ?

Milacron
 
Not exactly sure what you are trying to do.
Is this is a direct PC to control memory transfer , or are you trying to run using the DNC feature?

If its a straight file transfer then it is pretty straight forward.
First however you must have some sort of file transfer software on the PC.
You also need a cable that has the correct pin connections from the PC to the control.

You must have both the PC and the control set for the same transfer rate, number of data bits ,number of stop bits and what sort of parity you wish to run (odd, even or none)
My personal setup uses 4800 baud, 8 data bits , 1 stop bit , and no parity.

You need to have the file format exactly correct. The control is very fussy about the header and ending lines of the program or it won't accept it.

here is the basic setup:

(line1) $ or & %(then program number) "$" is inch program, "&" is metric program.
(line 2) space or line feed
(line 3)T# R# A L# A (Tool number, Radius value, allowance, Length value, allowance)

You need to repeat the above for each tool. One line per tool.

After last tool you need five (5) line feeds (returns)

Then : % (line following the five line feeds)
Next: ($ or & %#(program number) /000000)

Then your first program line.......

At the end of your program:
next to last line: ?
Last line: 0000

All lines start at the left edge of the page.

Here is an example from my CAM program ...I do not load any tool info at transfer, Keeps it simpler and i always need to set my
offsets anyhow, so i do that after the file is loaded and made active.

$%3
%
($%3 /000000)
N1 G0 X+0 Y+0 Z+4.
N2 G17 T73
N3 G0 G64 X-.0847 Y+0.8063 Z+1. F1.5 S+630 M8
N4 G0 Y+0.8063 Z+0.2
N5 S+630 Z-.1 F1.0
N6 G3 F1.5 X-.079 Y+0.7516 I+0.00N139 G0 X+0 Y+0 M7



N140 M30
?
0000

This is program 3 in inches....

To load the program into the control, you must go to mode 14.
Make sure there are no other programs in storage that have the same number as the one you are transferring.

At the control , be sure the control is set to receive....(IN)
Press the "Acknowledgement" and then the "transfer" keys.

Go to your PC and transfer the program.
You should see the block numbers going by on the control screen as they are loaded into the control.....

When the transfer is complete and there are no errors...switch to mode 13, highlight the loaded program and make it active by pressing the
acknowledgement key......

Cheers Ross
 
@ Milacron, yes the dialog 4

@Ross this is why i`m always reading all the topic overhere, Thanks for all the info.

I`ve already made the cable ( By reading other topics )
And i know the previos owner used the machine with a PC next to it ass well so all the opties should be ok.
Putted on 9600 7 and 1 that were the installed number so figured it worked that way. ( i will try yours if those won`t work )

Since i only have the manual for the controls up to switch 13 i really have no idea how to use 14 and 15.
So wich key is the "Acknowledgement" Thats the one with the J and the daimond ?
And wich one is then the "transfer" key ?

So then you should see it on the deckel control screen ?
On the pc screen its already sending but cant see if it goes to the deckel.
Will try it tommorow as i dont have time today.

Hope there are not to much questions...
But wath does the dnc mode does then >?

When i`m right i have a drawing program in 3D then can make an NC code special for the deckel ( Bought it this way )
The code seems to look the way you discribe it, will check that exaaclty tommorow ass well....

Thanks for all the help !
Keep you guys posted.

cheers Remco
 
Remco:

9600 baud will work, however it is sensitive to the cable length and "noise" in the work environment. On my machine running at 9600 causes data to get lost or corrupted
so i run a bit slower to avoid any issues on that score.

Make sure the cable is connected to both computer and control.
When in mode 14 press the "Acknowledgement" key. That is the button just to the right of the delete key. Should be white in color with the symbol being a diamond with a "J" on the
left side. (As in "Ja" )

When you press the Acknowledgement key the "IN" at the top of the screen should be highlighted.
There should also appear a white box lower middle of the screen with the characters; "%" "?".

Then press the transfer key....that is the green diamond symbol with a pointer on the left side. (lower right of the keyboard)

With the transfer key pressed, the screen on the control should now show:
In highlighted at the top left of the screen.
there should be a row of highlighted characters just below the in.
Characters should be: "%" "%*" "D" "T" and "P"

Just below that should be a white box showing "> % ?"

The control is now ready to accept data .....
Now you go to the PC and begin the file transfer...not before!

Once the transfer begins, the white box will be replaced by the line numbers as they are loaded into memory. (your program must have a number for each program line)

If the white box area does not display the numbers counting up, but shows something like ??? then something is wrong with the transfer or program syntax.


DNC mode is a method of running programs larger than the memory of the control/or greater than 9999 lines ..Need special hardware and software for that...
That topic has been talked about in some depth here on the forum....

Cheers Ross
 
I have atlast done the cable with ross example and It is working, but the lines with tool inputs and compensations isnt clear for me.

Does all the tool specs etc appear in the tool menu in dialog control?
It is impossible to read/edit the code what is transfered with the control?

Can you ross give an example of the code with 2-3 different tools? :)

The tool list etc is a thing which needs to be done always manually?
 
I never send tool data as part of the file transfer from computer to machine.....
Maybe i am lazy, but since i will have to set the length offsets using the machine , it means i am entering tool data manually in mode 10 so i just do it all at the same time. , i just enter the tool numbers and its offset MDI directly in mode 10 and i am good to go.

My CAM system "Post" that i wrote is without the tool data so it does not transfer any of that to the control.....
It is not hard to send the data, but as stated above , don't see this as any advantage ....
Tool information appears in the header of the transfer and like all things CNC and in particular Deckel the format is quite specific.

If you want to see what the format needs to look like...write a simple program at the control with tool data present in mode 10.

Then transfer that program to your computer. Use a text editor to view the result..Been so long since i transferred tool info i am not sure i could give you an accurate sample of the proper format.

Cheers Ross
 
If you want to see what the format needs to look like...write a simple program at the control with tool data present in mode 10.

Then transfer that program to your computer. Use a text editor to view the result..Been so long since i transferred tool info i am not sure i could give you an accurate sample of the proper format.

Cheers Ross

Here's one I output to a PC. Disclaimer, not my work, I didn't' see it run.

$%63

T1 R A L4.495 A (.375 E.M.)
T2 R A L4.72 A (.250 DRILL)
T3 R A L5.41 A (.343 DRILL)
T4 R A L4.68 A (CHAMFER)
T5 R A L16.6037 A (.375 E.M.)





%
($%63/000998"234P5055)
N1 G17 T1
N1111 G0 C0
N2 S+800 M3
N3 G55 W-60 I0 J0
N4 G0 X0.625 Y10.6647 Z1.55
N5 N*1 G0 X0.623 Y10.6647
N6 N*1 G0 X-0.627 Y10.6647
N7 G53
N8 G55 W-30 I0 J0
N9 L1 N4 N7
N10 G55 W30 I0 J0
N11 L1 N4 N7
N12 G55 W60 I0 J0
N13 L1 N4 N7
N14 G0 X10 C180.052
N15 L1 N3 N13
N16 S0 T0 M9
N17 G0 X12 Y0 Z12
N18 G0 C0
N19 M1
N200 G17 T2
N201 S+1600 M3
N2010 G0 C0
N202 G55 W-60 I0 J0
N203 G0 X0.625 Y10.7619 Z3.05
N204 N*2 G0 X0.625 Y10.7619
N205 N*2 G0 X-0.625 Y10.7619
N206 G53
N207 G55 W-30 I0 J0
N208 L1 N203 N206
N209 G55 W30 I0 J0
N210 L1 N203 N206
N211 G55 W60 I0 J0
N212 L1 N203 N206
N213 G0 X10 C180.052
N214 L1 N202 N212
N215 S0 T0 M9
N216 G0 X12 Y0 Z12
N217 G0 C0
N218 M1
N300 G17 T3
N301 S+1600 M3
N3010 G0 C0
N302 G55 W-60 I0 J0
N303 G0 X0.625 Y10.7619 Z3.05
N304 N*3 G0 X0.625 Y10.7619
N305 N*3 G0 X-0.625 Y10.7619
N306 G53
N307 G55 W-30 I0 J0
N308 L1 N303 N306
N309 G55 W30 I0 J0
N310 L1 N303 N306
N311 G55 W60 I0 J0
N312 L1 N303 N306
N313 G0 X10 C180.052
N314 L1 N302 N312
N315 S0 T0 M9
N316 G0 X12 Y0 Z12
N317 G0 C0
N318 M1
N400 G17 T4
N401 S+1600 M3
N4010 G0 C0
N402 G55 W-60 I0 J0
N403 G0 X0.625 Y10.6647 Z1.55
N404 N*4 G0 X0.625 Y10.6647
N405 N*4 G0 X-0.625 Y10.6647
N406 G53
N407 G55 W-30 I0 J0
N408 L1 N403 N406
N409 G55 W30 I0 J0
N410 L1 N403 N406
N411 G55 W60 I0 J0
N412 L1 N403 N406
N413 G0 X10 C180.052
N414 L1 N402 N412
N415 S0 T0 M9
N416 G0 X0 Y13 Z12
N417 G0 C0
N418 M34
N419 G0 Y21
N420 M1
N500 G18 T5
N501 S+630 M3
N502 G56 X0 Z-8.433
N503 G0 C30
N504 G0 X-0.1 Z6
N505 G0 Z0
N506 G0 Y1
N507 G0 Y0.1
N508 G1 Y-0.35 F20.0
N509 G1 Y-0.75 F1.6
N510 G1 X0.1
N511 G1 Z-0.0235
N512 G1 X-0.1
N513 G3 F1.6 X-0.1 Z0.0235 I0 K0.0235
N514 G1 X0.1
N515 G3 F1.6 X0.1 Z-0.0235 I0 K-0.0235
N516 G1 Z0 F20.0
N517 G0 Y1
N518 G0 Z6
N519 G0 C60
N520 L1 N504 N518
N521 G0 C120
N522 L1 N504 N518
N523 G0 C150
N524 L1 N504 N518
N525 G0 C210
N526 L1 N504 N518
N527 G0 C240
N528 L1 N504 N518
N529 G0 C300
N530 L1 N504 N518
N531 G0 C330
N532 L1 N504 N518
N533 S0 T0 M9
N534 G53
N535 G0 X0 Y21 Z12 C10
N536 G0 C0
N537 G0 Y13
N538 M35
N539 G0 Y18
N540 M30

N*1 G81 F4.0 S+800 Z-0.4 Z1.5
N*2 G81 F8.0 S+1600 Z-0.21 Z3.02
N*3 G81 F15.0 S+1600 Z-0.017 G4 F0 Z3.12
N*4 G81 F15.0 S+1600 Z-0.018 G4 F0 Z1.7

?
8231
 
A few additions to the above:

Mud's program:

1- this line: ($%63/000998"234P5055) Should read like this: ($%63/000000"234P5055) if sending to the Dialog control
2- "234P5055" is the program name and can use any standard letters, numbers or symbols. Letters can be upper case or lower case
3- Last line of the program needs to have "0000" on a new line that comes after the "?" line at the end. In my experience you need at least (2) blank lines (carrier returns) after the "0000"
4- The "998" and "8231" are checksums generated and used by the control- when you send a program those spaces always need to be "000000" in the program line and "0000" following the "?" --When you receive a program from the control, you will see different numbers in those locations (they are randomly generated)
5- Note the line format in Mud's program- it's important to have 2 carrier returns (line spaces) between the header and the tools, and 5 carrier returns between the tools and the main body of the program.
6- the "?" symbol at the end of the program can be on the next line immediately following the last block (no blank line(s) required)
7- the "T" lines are correct, but note that Mud is only using "length compensation" and "Length Compensation Allowances" in this program- no Radius Comp nor Radius Allowances. If you want to use Radius Compensation, just enter the tool radius after the "R"

The $ sign in the program tells the control the program is in inches.
 
A few additions to the above:

Mud's program:

1- this line: ($%63/000998"234P5055) Should read like this: ($%63/000000"234P5055)
2- "234P5055" is the program name and can use any standard letters, numbers or symbols. Letters can be upper case or lower case

IIRC the program name displayed on the control was "63" like in the first line above the tools. I don't understand the rest of the digits. "234P5055" may have been the part description displayed, perhaps a drawing or work order number..
 
Thank you all for your response! :)

First time i tried to send program to machine i had error 278 what is about Tool etc.
Then i added tool and program numbers etc before the code and Then it went through.

The First time i didnt have program numbers and metric signs etc before the program code. Maybe that is also a reason for the 278 error?

After that i had error 99 which says i have metric /inch conflict. I searched the text file for $ sign but didnt find one. And this i get in Mode 8 or 9.


"%" "%*" "D" "T" and "P"
What does these stand for?

Today or tomorrow ill go play more with these. This all New to me and Im way off my comfort zone.
This forum has been so helpful!
 
Post a photo of the screen in mode 8 or 9 showing the "%" "%*" "D" "T" and "P". also, we can help you better if you post your program here.
 
"%" "%*" "D" "T" and "P" is in mode 14.
Do i need to add lube cycles manually to the cam generated code?
Atleast there isnt any m7 commands.
 
When in mode 14 press the "Acknowledgement" key. That is the button just to the right of the delete key. Should be white in color with the symbol being a diamond with a "J" on the
left side. (As in "Ja" )

When you press the Acknowledgement key the "IN" at the top of the screen should be highlighted.
There should also appear a white box lower middle of the screen with the characters; "%" "?".

Then press the transfer key....that is the green diamond symbol with a pointer on the left side. (lower right of the keyboard)

With the transfer key pressed, the screen on the control should now show:
In highlighted at the top left of the screen.
there should be a row of highlighted characters just below the in.
Characters should be: "%" "%*" "D" "T" and "P"

Just below that should be a white box showing "> % ?"

The control is now ready to accept data .....
Now you go to the PC and begin the file transfer...not before!

Once the transfer begins, the white box will be replaced by the line numbers as they are loaded into memory. (your program must have a number for each program line)

If the white box area does not display the numbers counting up, but shows something like ??? then something is wrong with the transfer or program syntax.

Cheers Ross

Ross, I never knew to use the acknowledge key. I use only the transfer key in mode 14. Hit it twice and both the data and program get transferred. I just tried it again, and I can see no effect when I use the acknowledge key. Or the delete key for that matter. Every time I press transfer twice, the program gets sent from control to pc, even if there were some acknowledge or delete key presses in between. In mode 15, I hit transfer twice then delete, then paste the program into the pc's tty window. No acknowledge key needed. Did this behavior change from D2 to D3/4?

A related question: there are two acknowledge keys, the one next to delete and the one with a double rectangle, just to the right. What is the purpose of the second acknowledge key?

Dave
 
"%" "%*" "D" "T" and "P" is in mode 14. Do i need to add lube cycles manually to the cam generated code?Atleast there isnt any m7 commands.
"%" means "program"
"%*" is used for Macros - "%10" would be Macro #10
"D" is tool diameter
"P" is parameter

RimCanyonDave- only have experience with Dialog4, there are certain functions that are accessed using the Acknowlege key.

An example: managing RS232 interface in Mode 14- one uses the cursor to select "In", "Out", "RS232", then the Acknowlege key to confirm the selection.
This can't be done using the Transfer key.

Seems to help me to think of the Acknowledge key as the "minor enter" key and the Transfer key as the "major enter" key
 
I imagine this changed from D2 to D4. What about D3, is it the same as D2 or D4 in this respect? I am working on getting a D3 machine, but the D3 supplement to the operators manual does not mention any changes to modes 14 or 15. The one feature D3 has that I really want is the video tool path simulation.
 
Sorry, no help from here. Never used a D3 machine, no have i had a D3 operators manual so no idea of the differences there....
Suspect the D3 is close to the D2 in operation and features....
Think the huge difference between the D3 and D4 was the tool comp management which became more like other CNC controls on the D4 in that the comp was applied across the total program, not locally on each
block. Also as a side note, the D4 will happily accept D3 programs, which is why i believe it retained the "D" comp call within the programming structure.

Cheers Ross
 
"%" "%*" "D" "T" and "P" is in mode 14.
Do i need to add lube cycles manually to the cam generated code?
Atleast there isnt any m7 commands.


For my money you need to have lube cycles called within your auto programs....
The post processor i wrote for SurfCam always does a lube cycle at the end of all programs....Also at any rapid to the tool change point....

You can also just push the lube button on the control. You may do this any time, but it won't really do the cycle until the next rapid move!
The control will not allow lube cycles when moving using a feed move,linear, or circular.....

Cheers Ross
 
Okay, i need To figure out How to add it to fusion 360 post processor, also g18 adds would be nice... I am just tota newbie with these and only help i have had is PM and Im thankfully of that :)

If i remember right it also gives lube cycle when a dwell/stand still is programmed. This just doesnt spread the oil in the ways.
 
SurfCam prompts me when i go to post a program. Asks if the program is to be G17 (vertical) or G18 (horizontal)

But be aware that the machine sees the moves looking from the spindle, where most CAM programs only view things as though the part being run vertical.
Part of the issue is that Deckel does not rename the axis that carries the spindle unlike most machines....
So your CAM post must compensate for the change in orientation.
My post when running horizontal, inverts the signs (X*-1) of all "X" moves and components of "X" in canned cycles to agree with the way the program is viewed.

Cheers Ross
 








 
Back
Top