Dialog 4 - error 70

Hello,
I'm spinning in a circle and can't get out of it.

Problem: I was sending G-code into Dialog 4. After the sending was done I switch from program BA14 on to BA9 an error occurred (error 70), pressed "?" typed N1, N2, N2, ...etc. to check if the code was there and everything looked OK. Switched to BA10 too check the tool and this is where it gets freaky. Tool interface isn't there, no tools are shown, BA11,12,13 same story. In BA13 I can't delete anything. The program that I loaded was named "P3" (&%P3) in BA13 there was none, only "%". I try to delete it but with no success. Prior to this problem, everything was normal.
Is there a solution for this?

Backstory: I was learning how to use and test the machine because I bought it a few months ago. X, Y, Z axis worked fine, spindle worked fine as well so it was time to learn how to work on the machine. Especially post process and "drip feed" with AutoDNC.

Information:
- Deckel FP5 NC (y. 1985)
- Dialog 4

- AutoDNC
- Windows 10

- error 70 = NC-program is empty

For the post process, I'm using:
- Autodesk Inventor 2020 + HSM

Can I get some information about AutoDNC how to use it properly because for now, the only way to send data in was with HSM?

And does anyone own a copy of Dialog 4 book in English? I only have the German version.

Best regards
Domen Matevzic

Questions:
Have you ever been abler to send or transmit programs form that machine to a computer?

AutoDNC only works if your machine has the needed software installed along with the needed hardware option.

Need to turn to mode 16 and hit the "info" key to see the software version you have loaded....You must have "Package 3.07" or the
DNC feature will not work.

Need to have a proper cable (RS232 ) to send and receive from the machine.

The screen shot you show for mode 10 looks like its for setting offsets using the local tool comp "D" values. These are local comp values generally associated with earlier (D3) programs.
For Dialog4 programs your tool comp page should list each tool number , a radius value and a length comp value.....Along with an "A" (allowance) value for each......

Can you post a copy of the program exactly as you attempted to send it?

AutoDNC i believe requires a hardware "Dongle" (key) in order to work. Is this device connected?
Is your AutoDNC windows or DOS based (they made both)

Pretty sure you don't need the "P" in your program label....Might be an issue...The control is very specific about the syntax of a sent program, the format must look like this:

$ or & %(program number ) The "$" is for inch programs, the "&" is for meter programs
Space or line feed........................
T#................. R#............... L# A#
Repeat tool format for as many tools as being used...one tool per line....Tool number 1-9999
Space
Space
Space
Space
%
($ or & %#/000000 comments here if any)
N1 Go X0 Y0 Z4.0 first line of program.....
N2 G17 T1............
...........
................
N100 M30 (last program line)
?
0000

You can omit the tool lines and just start the download at the "%" line, then enter the tool info manually when you set the tool lengths at the control....
Does your AutoDNC even open and run under Windows 10?

Cheers Ross

You probably have some bum characters, or are lacking necessary characters, in the file you are sending. Dialog 4 is sensitive that way, to say the least. For example, each tool table line needs to end in a space character and then the return character. You need five "blank" lines after the last tool line in the tool table, and the "blank" lines are not really blank; they need to have a space character in addition to a return character. I have encountered these and similar issues over the years. Often, the only recourse is to reboot by pulling the K10 jumper and X120 connector inside the console. See here where Ross explains how.

PM me your email address, and I will email you a short g-code text file in the proper format, so you can see what characters and spacings are needed.

OK read your post again...i see that your have 3.07 software....OK....
Screen shots show Dialog3 program that is why there are no "T" values in your tool store....the control is asking for tool 1 , its not there.
The reason you can't delete the program is that its not there...the storage value is not changed, no data has been used...

AutoDNC works by first turning it on at the control.
Go to mode 14 and key to "RS232"
Key "acknowledge" (the "J"within the diamond key)
key down the list to "DNC"
Using the right or left key change DNC to "On"

Select mode 15 send split program to begin DNC operation....
Note:
The Dialog DNC is not drip feeding. How it works is that first you must prepare a program .
That consists of splitting up a large program into smaller files that are flagged with sequential headers and footers .
These smaller programs are then sent in order to the control. AutoDNC will send as many programs as there is memory available in your control.
As the programs get executed in order, each used small program is deleted to make room for loading memory with more....
This process continues till the entire set of small programs have been run.....

Aurto DNC controls the flow rte to the control, the control controls the request for more smaller programs as it has room. The control controls the deletion of the used programs once they have been run....

When you first start the DNC using "AutoDNC" you request the first file to be sent using the control.
The request needs the "%" and a four digit file number which must be present in the AutoDNC folder.

Once requested (if all is correct) the computer will begin sending the first file.to the control
Once that file has been sent , you switch to mode 13 , and you will see the first file number that you requested. Make that filer active by selecting it.
You may now go to mode 10 and enter your tool numbers and offsets.
Then you go to mode 9 , assuming the first tool is in position and begin running the program under automatic operation.....

The above is a general overview assuming that AutoDNC has been setup correctly , that the communications are correct and the program has been split and stored in the correct folder....

Some of this is a bit fuzzy to me as i haven't used the DNC setup on my machine in some time.....Hope some of this helps....
Cheers Ross

Hello,

so I hard reset the machine by pulling K-jumpers from the panels (thank you rklopp). From now on the machine is working fine. The error happened because in the post-process I forgot to put a program number behind %.

AutoDNC is working on Windows 10 (so I thought). It opens up and all but I cannot enter any programs. Need to look into it why.

For now, Autodesk HSM is working kinda well. Programs are transferring as normal and I can run them. When I said kinda I meant this (I posted this): Dialog 4 combine G1 and G2-G3 movement - Autodesk Community

Thank you for explaining how AutoDNC works and for the useful information!

Best regards
Domen

Looked at your posted code...Some confusion on my part....
Stuff there i do not understand
First off the program number should not have "P" within it.....
Forget all the uses of "D" within the program...that is Dialog3 verb age and suspect confuses the control.
Simplify the loaded format...omit the tool information. You can enter the tool offsets manually after the program has loaded, you need to set your tools relative to the part so enter the info directly in mode10
and forget entering that data in your post....

Begin the program numbers at the first real machine move....
For all my programs the first line i always use is a GO to rapid to X0.0 and Y0.0 and Z4.00 (clearance for tool change) when running vertical in inches..

With tool info omitted the program looks like:
%
($4%#/000000)
N1 G0 X0 Y0 Z100
N2 G17 T1
N3..............

Dialog4 does not need a "G1" to do linear interpolation so long as you have defined a feed rate! Any axis move is assumed to be a linear move unless otherwise defined.
Feed rates are modal.
Rapid moves must be called every time they are used...
Again , loose the "D" values, that will only confuse the operation. D values are "local" comp calls that apply offset at the line where called, but they compound to any standing tool offsets as defined in the
tool offset page (mode 10)

No reason that linear and circular moves can't be called in the same program.....Just need to be sure you are defining the curve correctly.

Line 14 you call G18....Length comp in the "Y" (horizontal) then in line 16 you call out a G17 (length comp in the Z, vertical)....Can't mix vertical and horizontal calls in the same program...
Define the working direction early in the program and leave it alone....Choose one orientation and only the appropriate "I","J" and "K" call outs when doing circular cuts....

Don't see any call for the tool "T" in the first program. Again here using the "D" call only applied to the block where written.
Can't tell about the use of the G2/G3 without a drawing...

Can you get to the post programming portion of your program...Must be a section where you set the machine specific needs....a sort of fill in the blanks file that controls how your post functions...

Starting at line 17 you have "I" and "J" values , but the moves are linear . Those I's and J's have no effect on a linear move and shouldn't be there.Seems that your post carries the I's and J's down the program, don't understand what or why they are there.

Line 16 calls a circular move, but that should be complete in a single line. Should not include a linear move (G1) on this line if the intention is to cut a curve.
If your program is doing a 3-D surface using small linear moves (like most CAM programs do) it should not be using any "I's or "J's"


Sure there are lots more things here that i don't see at a glance....
Cheers Ross

I think you misunderstood the post. If not correct me.

The link that I send is for a problem within the post-processor. In the picture, you see the same program. One is named 4.nc and the other 41.nc.
- 4.nc is the default post-process I get before editing.
- 41.nc is semi-edited.

This program was written for bore milling 2 holes. And this is the problem with my post-processor. It dosesn't understand G3 (or helix movement). It outputs G3 only in one line then all the other lines are without the G3 function. The machine makes one circle and the following steps are linear. I got around this by manually write G3 in-front of the lines. But when it comes to bigger products it is time-consuming and I was looking for fixes within the post-processor.

Found one fix but it was lacking G1 movement for some reason which was hell in its own way.

I'm interested, what programs for post-process do you use?



One thing the machine is doing is stop-and-go motion. Every line that is completed the machine stops for a split second and proceeds to the next one. Is this normal or is a problem with overflowing the Dialog with information because of high-feed rates?

I have a lot of questions so apologise for not sticking to the point.

Best regards
Domen

Thanks for the clarification!
Some notes:
The CAM program i use is SurfCam. My program is a number of years old (not the most current.
I was a registered user for years on maintenance and all...Let it lapse so now i am on my own.

Program has its own communications sub program that runs under SurfCam.
The post i have was a generic post supplied from SurfCam, that did not work at all.
I rewrote the post to make it work for me.
The program allows posting for either vertical spindle or horizontal as needed (i run both about 60/40)

Don't see why you are using the "D" values.....
As stated earlier, you can't mix G17 and G18 in the same program....don't understand why your post does that.

As to stop and start....many short moves will cause this ..Accell and decell takes time and the Dialog does not have much look ahead so it can't predict where the next move will take it and so
compensate on the current move...result is a herky -jerky move...

You can help this by forcing the control to "average" start/stop points...sort of blend..
Get your post to insert a G64 at the start of your program...it will help.

Need to figure out why the post is inserting linear (G1) moves along with circular (G2) moves....this is just wrong (line 14,16)

Having a depth move (Z) as part of a circular move in Dialog4 will produce a helical cut. Depth will be cut in the course of doing the curve that was programmed.
If you want to make circular cuts in steps, then your post must have a stand along depth move before each curve move....
Note: Early software versions of Dialog4 won't do helical cutting....

Saw your note about finding a "fix" but it did not have the "G1" Remember that you do not need to write "G1" to execute a linear move....It is always assumed as long as you have a feed rate set somewhere before the
linear move is called. Point is that the fix might be fine.

Cheers Ross

As a point of interest here are the vertical and horizontal posts for my Surfcam.
These are in effect definitions that the poet uses to output code that works....
Somewhere in your CAM there is a similar file and it is where you can direct the post to make good code.....

name Deckel Dialog 4 Plane G17

! 00
% >4
b >4
Q 00
N >5
G >2
f >3.1 F
s +->4 S
X +->3.>4
x +->3.>4 X
Y +->3.>4
y +->3.>4 Y
o +->3.>4 Z IncFrom V
q +->3.>4 mult -1
a +->3.>4
z +->3.>4 Z
g >2
r >3.>4
e >2.1
c >3.>4
u +->3.>3 add -2
Z +->3.>4
F >3.1
S +->4
I +->3.>4
J +->3.>4
K +->3.>4
B +->3.>4
T >2
M >2
V 0
W 00
O 00
w >4
P 00
$ 00


Leading0s? N #print leading zeros

ModalLetters X Y Z F # List of letters that are modal

ModalGs 1 90 91 # List of g codes that are modal

Sequence#s N 1 1 1 # Char, freq, incr & start

First#? N # Y or N 'Output 1st sequence no.
Last#? N # Y or N 'Output last sequence no.

HCode X # X or X U 'Horizontal char.
VCode Y # Y or Y V 'Vertical char.
Dcode Z # Depth char.
FeedCode F # Feed rate char.

Comment ( ) # Begin End comment char.

Sbackdoor supressheader

Spindle 3 4 5 # Cw, ccw & stop m codes
Coolant 8 9 8 # On, Off & Mist m codes
DComp 41 42 40 # Left, Right & Cancel m codes
LComp 43 49 # On & Off codes
Rapid G0 # Rapid positioning word

Spaces? Y # Y or N 'Spaces between words
Incremental? N # Y or N 'Inc or abs output
CtrIncremental? Y # Y or N 'Inc or abs I & J
ByQuadrants? N # Y or N 'Break arcs at quadrants

Inc/Abs G 91 90 # Inc & Abs char. & values
Helical? Y

UppercaseComments? Y # Y or N 'Require uppercase comments

Drill 4 # Drilling canned/manual cycle
G0 x[H] y[V] z[Rplane]
G0 z[VClear]
G81 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 z[Rplane]
end

Peck 4 # Pecking canned/manual cycle
G0 x[H] y[V] z[Rplane]
G0 z[VClear]
G82 f[Frate] s[Speed] V[VClear] o[D] q[VBite] a[.015] e[Dwell]
G0 z[Rplane]
end

Custom1 # Deep hole canned/manual cycle
G0 x[H] y[V] z[Rplane]
G0 z[VClear]
G83 f[Frate] s[Speed] V[VClear] o[D] q[VBite] a[-.015] z[-.002] e[Dwell]
G0 z[Rplane]
end

Tap 4 # Tapping canned/manual cycle
G0 x[H] y[v] z[Rplane]
G0 z[VClear]
G84 f[Frate] s[Speed] V[VClear] o[D]
G0 z[Rplane]
end

Ream 4 # Reaming canned/manual cycle
G0 x[H] y[v] z[Rplane]
G0 z[VClear]
G85 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 z[Rplane]
end


Bore 4 # Boring canned/manual cycle
G0 x[H] y[V] z[Rplane]
G0 z[VClear]
G86 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 z[Rplane]
end

Cancel # Cancel a canned/manual cycle
G80
end

StartCode
!0 w[Program#]
!0 P0
!0 b[Program#] Q0
end # START OF PROGRAM

1stToolChange
G0 x[0.0] y[0.0] z[ToolD] # First tool change
G17 T[Tool]
G0 G64 x[H] y[V] z[D] F[fRate] S[Speed] M[Cool]
end

Infeed # Enable cutter comp
G[Side] T[TOOL] h45 A0 X[H] Y[V] i01 j60 M60
G1 Z[D] F[Plunge]
G[Side] X[H] Y[V] f[FRate]
Upon [Speed]
S [Speed]
end

Outfeed # Disable cutter comp
G40
G1 X[H] Y[V]
end

ToolChange # Secondary tool changes
G0 z[ToolD] M9
G17 T[Tool]
G0 G64 x[H] y[V] z[D] F[fRate] S[Speed] M[Cool]
end




EndCode # End of the program
G0 Z[ToolD] M9
G0 X[0.0] Y[0.0] M7
M30
!0 W0
!0 O0
End

LineCode # Linear move
X[H] Y[V] Z[D]
end

RapidCode # Rapid move
G0 X[H] Y[V] Z[D]
end

CwCode # CW circular move
G2 f[FRate] X[H] Y[V] I[IVal] J[JVal]
end

CcwCode # CCW circular move
G3 f[FRate] X[H] Y[V] I[IVal] J[JVal]
end

Replace "g" with "G"
Replace "r" with "F"
Replace "o" with "Z"
Replace "q" with "Z"
Replace "a" with "Z"
Replace "u" with "Z"
Replace "c" with "Z"
Replace "V" with ""
Replace "b" with "($%"
Replace "Q" with "/000000)"
Replace "W" with "?"
Replace "O" with "0000"
Replace "e" with "G4 F"
Replace "P" with "%"
Replace "w" with "$%"




name Deckel Dialog 4 plane G18

! 00
% >4
b >4
Q 00
N >5
G >2
f >3.1 F
s +->4 S
X +->3.>4 mult -1
x +->3.>4 X
Y +->3.>4
y +->3.>4 Y
o +->3.>4 Y IncFrom V
q +->3.>4 mult -1
a +->3.>4
z +->3.>4 Z
g >2
r >3.>4
e >2.1
c >3.>4
u +->3.>3 add -2
Z +->3.>4
F >3.1
S +->4
I +->3.>4 mult -1
J +->3.>4
K +->3.>4
B +->3.>4
T >2
M >2
V 0
W 00
O 00
w >4
P 00
$ 00

Leading0s? N

ModalLetters X Y Z F # List of letters that are modal

ModalGs 1 64 90 91 # List of g codes that are modal

Sequence#s N 1 1 1 # Char, freq, incr & start
First#? N # Y or N 'Output 1st sequence no.
Last#? N # Y or N 'Output last sequence no.

HCode X # X or X U 'Horizontal char.
VCode Z # Y or Y V 'Vertical char.
Dcode Y # Depth char.
FeedCode F # Feed rate char.

Comment ( ) # Begin End comment char.

Sbackdoor supressheader

Spindle 3 4 5 # Cw, ccw & stop m codes
Coolant 8 9 8 # On, Off & Mist m codes
DComp 41 42 40 # Left, Right & Cancel m codes
LComp 43 49 # On & Off codes
Rapid G0 # Rapid positioning word

Spaces? Y # Y or N 'Spaces between words
Incremental? N # Y or N 'Inc or abs output
CtrIncremental? Y # Y or N 'Inc or abs I & J
ByQuadrants? N # Y or N 'Break arcs at quadrants

Inc/Abs G 91 90 # Inc & Abs char. & values
Helical? Y

UppercaseComments? Y # Y or N 'Require uppercase comments

Drill 4 # Drilling canned/manual cycle
G0 X[H] y[Rplane] z[V]
G0 y[Vclear]
G81 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 y[Rplane]
end

Peck 4 # Pecking canned/manual cycle
G0 X[H] y[Rplane] z[V]
G0 y[VClear]
G82 f[Frate] s[Speed] V[VClear] o[D] q[VBite] a[.015] e[Dwell]
G0 y[Rplane]
end

Custom1 # Deep hole canned/manual cycle
G0 X[H] y[Rplane] z[V]
G0 y[VClear]
G83 f[Frate] s[Speed] V[VClear] o[D] q[VBite] a[-.015] z[-.002] e[Dwell]
G0 y[Rplane]
end

Tap 4 # Tapping canned/manual cycle
G0 X[H] y[Rplane] z[v]
G0 y[VClear]
G84 f[Frate] s[Speed] V[VClear] o[D]
G0 y[Rplane]
end

Ream 4 # Reaming canned/manual cycle
G0 X[H] y[Rplane] z[v]
G0 y[VClear]
G85 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 y[Rplane]
end


Bore 4 # Boring canned/manual cycle
G0 X[H] y[Rplane] z[V]
G0 y[VClear]
G86 f[Frate] s[Speed] V[VClear] o[D] e[Dwell]
G0 y[Rplane]
end


Cancel # Cancel a canned/manual cycle
G80
end


StartCode
!0 w[Program#] # Start of the program
!0 P0
!0 b[Program#] Q0
end

1stToolChange # First tool change
G0 x[0.0] y[ToolD] z[0.0]
G18 T[Tool]
G0 G64 X[H] y[D] z[V] F[FRate] S[Speed] M[Cool]
end

Infeed # Enable cutter comp
G1 Y[D] F[Plunge]
G[Side] X[H] Z[V] F[FRate]
Upon [Speed]
S [Speed]
end

Outfeed # Disable cutter comp
G40
G1 X[H] Z[V]
end


ToolChange # Secondary tool changes
G0 Y[ToolD] M9
G18 T[Tool]
G0 G64 X[H] y[D] z[V] F[FRate] S[Speed] M[Cool]
End

EndCode # End of the program
G0 Y[ToolD] M9
G0 x[0.0] z[0.0] M7
M30
!0 W0
!0 O0
End

LineCode # Linear move
X[H] Z[V] Y[D] F[FRate]
end

RapidCode # Rapid move
G0 X[H] Z[V] y[D]
end

CwCode # CW circular move
G2 F[FRate] X[H] Z[V] I[IVal] K[JVal]
end

CcwCode # CCW circular move
G3 F[FRate] X[H] Z[V] I[IVal] K[JVal]
end

Replace "g" with "G"
Replace "r" with "F"
Replace "o" with "Y"
Replace "q" with "Y"
Replace "a" with "Y"
Replace "u" with "Y"
Replace "c" with "Y"
Replace "V" with ""
Replace "b" with "($%"
Replace "Q" with "/000000)"
Replace "W" with "?"
Replace "O" with "0000"
Replace "e" with "G4 F"
Replace "P" with "%"
Replace "w" with "$%"




Cheers Ross

PM me your email address, and I will send you a .cps post that works and handles G1, G2, and G3 just fine, and also G41 compensation on a contour.

The jerky movement is because the Dialog 4 has a 1986 computer! As Ross says, G64 helps. (I did not know you could use it outside of a G41/G40 contour compensation path, however. Ross, does G64 work anywhere?)

I always get smoother running code when I code by hand ("Finger-CAM"). Make sure to turn on "Smoothing" in your CAM so the post breaks curves into best-fit arcs, rather than gazillion tiny linear moves.

Does Autodesk HSM use the same post as Fusion 360? If so, it is written in JavaScript and pretty easy to debug and modify yourself. If you've ever tried to modify a Mastercam post, you'll appreciate how easy Autodesk makes it.

Can't reminder where I got the one I started with but it's now heavily modified. The ones available from Autodesk do a lot of things wrong. I'd send you mine but it still does a few things wrong* and I'd feel bad causing a crash.

Teryk

* Trying to remember but I think it gets the Z depth wrong on the circle milling canned cycle. I also only post in metric so haven't tested the inch stuff in awhile.

Sent from my XT1710-02 using Tapatalk

My understanding is that Fusion & HSMWorks use the same posts.


Sent from my iPhone using Tapatalk

rklopp said:

G64 helps. (I did not know you could use it outside of a G41/G40 contour compensation path, however. Ross, does G64 work anywhere?)

.

Click to expand...

Rich:
To tell the truth i can't answer that. I insert the G64 in most code that is CAM generated. But i never have confirmed that it is making a difference when running without diameter cutter comp (G41)
Honestly it never occurred to me that it would not be applied everywhere, but now that you mention the question i have doubts....
Need to make a test i guess.....
Cheers Ross

Thank you Ross for the information.
D values are automatically written by the post. Today I try deleting then out of the post and it helped.
I called G17 because the post didn't but the G18 was again written automatically. Don't know why. I checked the orientation in CAD and was ok. Will delete it out.

When you said, "inserting linear (G1) moves along with circular (G2) moves". It is trying to make a 1/4 circle motion along the Z-axis. I will post a picture of what I mean. But it is a jerky movement only in the "fix".cps is used properly.

Best regards
Domen

Picture for the 1/4 circle movement along the Z-axis.


The next few pictures are the result of helping me. A small step but never the less.

Domen:

My guess is that the post is entering "D" values because perhaps that post might really be for a Dialog3 control....Software authors , even relatively literate machine guys don't know squat
about the Dialog controls or Deckel operations in general....
Old obsolete control coupled to a machine that has little population out in the machine world....In reality nobody cares.

Programmers can fix or write a new post , but you have to pay to get any real help from the commercial outlets.
Even if you were willing to pay, you would need to run as many different programs using all the different features and operations so you could know what specific errors their current post generates.
Otherwise you would have to keep coming back for corrections ($) when a new operation or cycle did not produce the needed code.

Cheers Ross