Need Dialog 3 Subroutine/cycle/nesting help.

Hi all,
As I mentioned in another post, somehow in moving, my Dialog 3 programming manual has vanished. We've looked high and low but no luck. It was probably the last thing I was reading before moving so it hasn't turned up in the regular places.

I do have a Dialog 2 programming manual, and most all of it pertains, but I am having problems getting the correct format for the subroutine/cycles to work.

In the Dialog 2, you can simply type a line number with the subroutine number....

N0100 U0001
U0001 (Cycle)

or....

N0100 U0001
U0001 G81 S+1000 F34 Z-10000 (drilling cycle/speed/feed/depth)

Even G87 commands (subroutine) including the U0001 shut down the machine once the U0001 is called...with no error.

I think I recall something being a bit different in the format from the D2 to the D3 and this may have been it, but I'm stuck.

Could anyone scan/email, or type out the basics of the canned cycles/subroutines for the D3 or possibly the D4?

And on that note, does anyone have a D3 manual either hardcopy or electronic to sell?

Many thanks.
Sean

does anyone have a D3 manual either hardcopy or electronic to sell?

Click to expand...

I have a D3 manual and may even have an extra one...will try and look today.

"electronic" ?? You mean there may be someone out there nutty buddy enough to have scanned the gazillion pages to a CD ?

Don, you have mail.

This is how my week is going...
I am having similar problem as "crazykeith" is in this post...

Similar Problem

Of course, I don't think we've heard from that poster in quite awhile and though he says he fixed it, he doesn't bother to say HOW.

In addition to not getting the subroutines right, If I manually type in just a drill cycle (one block only) on the control...

N100
G81
F100
S+1000
Z-20000
(sequence, cycle, feed, speed, drill depth 2")

...the program works perfectly. It only requires one block and will do the cycle from wherever the tool happens to be.

Now if I type exactly the same thing in a text editor...

N100 G81 F100 S+1000 Z-20000

... and send it via serial, it comes up on the control looking precisely the same as if I had punched it into the control...

N100
G81
F100
S+1000
Z-20000

Hit "cycle start" and.....NOTHING. No errors. It is as if you programmed X0 Y0 Z0 *from* X0 Y0 Z0 and hit start.

The only difference I can think of is that when you type it into the control...being a canned cycle... it also prompts you for Dwell (V) and Safety plan (Z again). On the control, if you dont need these values, you hit the "Transfer" button to "Skip" them when asked. It does not present any value when "Skipping", the field just disappears and the end result is exactly as I typed above.
I have no reference (without the manual) on how to try to enter null characters or V (dwell) via text/serial, but it doesn't come up with any value missing errors.
I'm stumped.

Sean

Well no response so far. I think Ross is out having a BBQ (as he should be).

I've now been able to get the drill cycle to work, but only as a subroutine.

That would look something like this:

N100 U002
U002 G81 F37 S+1000 Z-10000

Oddly, when programming at the control, you do not need to do this. You can simply assign the line number to the cycle....

N100 G81 F37 S+1000 Z-10000

Now I'm getting back to the fact that when programming at the control and starting with line number, it asks you for V and Z(2) values which you can "skip" by pushing the transfer key.

I have no idea how to make it "skip" these values via the serial port, nor why it doesn't care if they are missing when you put the cycle into a subroutine (should do the same thing...no?).

This is seeming like a software (Grundig) bug.

It sure would be nice to be able to add a couple characters to the txt to have it take the cycle without a subroutine since it would save ram, save clutter, and ease programming.

Ideas?
Sean

FWIW, the D3 supplement manual says that operation and program input are "absolutely identical" on D3 and D2, but a variety of programming facilities have been added on D3.

Pockets with irregular external contrours can be programmed as 'contour pockets' Thread milling cycles have been incorporated to simplify machining of large diamter internal and external threads. Graphis display added also.

Thanks Don, that *is* worth something.

I'll be sure to post the result when I get it working.

The manuals I have don't state that you cannot program a cycle out of a subroutine. That may be the case, but it seems weird that you access the cycle directly via input at the control, yet not be able to access unless contained in subroutine if programming via RS232 input. I was hoping there'd be a note somewhere that addressed that with a "no way", or a "do this". If it is in the D2 manuals, I have yet to find it, but I don't recall the D2 being able to access them directly and the D3 can, so I thought maybe it was a series thing.

Beyond that, using the subroutines, I'm still having trouble getting them to return to the call line and continue the program, but I think I'll figure that one out with some more dart throwing.

Sean

Of course you may have the D3 "ME" edition which is way different !

Don, you and I have 2 different 2-character, capitalized characters that are going to kill us... For you it is "ME" and for me it is "CD"... Both kinda rhyme in a sick sort of way!

Actually, I have scanned many of the CNC manuals, but I do not have much specifically for the D3. It seems like most of my stuff is for the D2. I do have a programming manual for the Dialog 4, however, if that will help. There is patently *no* way I can email it though. It is 95Meg big. I also have 65 page Dialog CNC tutorial, although I cannot tell you the exact model it is for. That weighs in at a hefty 110Meg.

If there is something there that can help, let me know...

--Alan

Don, my darned life is the "ME" version. Never any good reference for it.l

Alan, I have high speed. Maybe you or I could do an FTP? I appreciate the offer and would be willing to try when you have time.

For now, what I am most humbly requesting is:

Anyone with a D1-D4 type this drilling cycle line solo in their control:

N100
G81
F50 (prompted)
S+250 (prompted)
Z-10000 (prompted...make sure you have 1 inch of Z clearance)
V (transfer key) (prompted, push transfer to "skip")
Z (transfer key) (prompted, push transfer to "skip")

Now run the program. It is a drilling cycle so it should advance the table towards the spindle (please no tool) @ 5in/min from wherever it started until it reaches 1in below wherever you started and Z rapid back to wherever you started.
This is an INCH program for reference. The cycle is incremental, the Z will "close up" by 1 inch so watch your collisions.
In addition, the D3 (as well as the D1-D2) don't use decimal points, so if your control does (D4+.. likely Contour), you would enter that as 1.0000 or 1.0. DO NOT forget that point and enter your drilling depth as -10 thousand inches (if it will even let you).
Keep your hand on that E-stop please! (I wonder how many D4/D11 users got bitten by this when used to programming without a decimal point on older Dialog controls?)

Anyway, the D3 will do this...not sure if the D2 will (as written).

Now, can anyone do the same thing via RS232 (serial)?

I'm most interested to see if a D2 owner can do it at all (via regular sequence number), and if the D4 owners can do it via the serial port using "N" numbers. I've seen that D4 owners can do it using N* numbers (love to see an example).
Maybe the D2 can do it from the control...I just can't remember.

In any case, the line via RS232 should look something *like* this (because this does not work for me):

N100 G81 F50 S+1000 Z-10000

Also, does anyone know the character for Dwell on the Dialog? I'd love to try to append a V0 and Z0 at the end of that line to mimic the "skipping", or a character to mimic the transfer key?

I've found very little documentation on the hidden (ctrl-ish) characters that the Dialog will recognize. Is there a list somewhere?

Many Thanks
Sean (soon to be expert....mmmmm)

OK, HOLD THE PRESSES!

As you may witness by the hour I am typing this, I have not been able to let this thing go in defeat.

Here's the scoop. It may mean nothing to those who by chance already use this format, but everything to those like me who can't figure out why the hell the subroutines won't work....

Anyway, the answer iiiiiiissssss....

Line number format.

While most everything will run using different line number formats (1, 01, 001, 0001), cycles and subroutines REQUIRE 4 digits if transferred via RS232.

I did not have my post processor formatting with leading zeros, so it would call a sub or cycle unders say...line 160 (N160) instead of correct (N0160).
No 4 numbers, no workie even though it works for everything else (linear moves...etc), and properly sequences it (10, 20, 0030, 040, etc.)

I would go and hand type it at the control but even though the control displays exactly what I enter (N160), it somehow internally converts that to "N0160" in its memory....and Yes Workie. Again...it doesn't convert to 4 digits via RS232 regardless of the display and ordering.

In addition, the subroutines must also be 4 digits if they come in via serial. Manual typing in the control will convert them (not visually), but not via serial, so type U02 at the control and it is displayed as "U02", you can even do a line search for "U02" and it will find it. Same search for "U0002" still finds it, but send "U02" through the serial port and it is not converted to memory as "U0002" even though the searches still work.
Searching seems unconcerned with leading zeros...it converts whatever, but actually jumping to and from that cycle/sub does not convert.

Anyway, you can do an awful lot of milling without using the canned cycles, and it is easy to get in the habit of less than 4 digit sequence numbers only to be suprised later that your sub's and can's don't work right.

The easy way is simply to make sure that both your sequence numbers and your subroutine numbers are 4 digits (D1-D3, not sure on D4) if you are using RS232 to transfer your programs.

Even the straight N**** (cycle) lines now work from the control with no subroutine (N0010 G81 F50...etc).

Type N10 G81 at the control >works
Send N10 G81 via serial >no work
Send N0010 G81 via serial >works
Etc.

You cannot believe how much analysis and dart throwing it took to figure this out since it is not in the (or my) manual, and for everything besides canned and sub's, it doesn't matter.

Many Thanks to everyone and I hope this can help somebody down the road.

Sean (ZZZZzZzZzzZzzzzz)

Sean:
Nice work! For infornmation the D4 as far as i know does not require the leading numbers to make the line number equall 4 digits. In fact the D4 will allow the use of the same line number more than once (but you must be careful if you are doing an unconditional jump or a loop and repeat as you may get the control to jump to a line number you did not expect.
Also it ahould be noted here that the serial imput by passes some other control safegards. On the D4 it is possible to have 2 programs of the same number in memory. If you enter one program MDI on the control and then send another with the same number the control will accept it and you could have two number one programs in memory. Might be like your expirence with the leading zeroes...possibly the manual program has the leading characters just not shown so the control does not see the conflict with the sent program.....
I am told that a D4 will run and accept D3 programs without any problem...never tried it but the decimal point thing would make some conversion necessary.

Good to see you working out the programming and the control. This is exactly what i did with the D4..took some time to get ti figgured out to the point that i felt comfortable with all the cycles and syntax. The manual can explain just so much...and for the D4 there was no information on the peramiter programming at all (hav some now). Of course now using a CAM proigram i have forgotten all that stuff, and i just have gotten lazy and let the computer do it long ways without sub routiens, macros or preamiter programming...just does not matter if you have DNC
Of courese now with two D2 machines in the house, i will have to become better at all that stuff again.
Keep up the good work..
Cheers Ross

On edit: I want to thank you Sean for the insight into the D3 control! Just walked over to my trusty FP4NC and powered up the control to make ready for another day of making "widgets"...found myself thinking "how lucky i had been to begin my Deckel CNC excpirence with a D4" It was just luck i suppose, but i am pretty happy it went that way for me. Almost bought a Tree Journeyman with a Delta control...would have taken me to a completely different place, and i fear i would not still be running that Tree today!

WRT the matrix project.... This seems like a good thread to ask a question, as the machines are still in your head(s)... Would you like to detail the differences between the D1, D2, D3, D4 and D11 machines all in one spot?

Thanks,
Alan

Alan: that is a great idea, but the trouble is that only person that posts regular here that has a D11 is Don T which means we will have to wait for about two years for him to get around to actually programming and using that control (he's a very busy guy looking for Euro machines that are fitted with color LCD readouts....)
Course we could just wait until someone on this board buys the FP2A and actually runs it for a report...(yea i know Don says that the machine is not for sale..but we know different )
At any rate Sean is giving some pretty good information about the D3 here and that is a good thing. Anyone out there really running a D2 machine??? Come on guys don't be bashfull, your imput is wanted.
Cheers Ross

Ok, well i just sent out an email describing the "restriction" to a person who was helping me via email.
I'll copy it here as it is another way of saying what hopefully I already said above (can't have too many versions with how I write).

**********
The short (and undocumented by Deckel) answer is that you can type in the control most all line number formats (N1, N01, N001, N0001, all equal "line 1").
You can do the same sending a text file via RS232 for all features *Except* canned cycles and subroutines, which *must* have a 4 digit line number (N****) and a 4 digit Subroutine (U****).
You can actually mix and match...as long as the cyc/sub numbers have four numbers:

N010 G00 X+10000 Y+10000 (Linear Move)
N20 G0 T01 (tool change)
N030 S0 (spindle stop)
N0040 G81 F50 S+1000 Z-10000 (drill cycle....MUST use N1234 format)
N45 G90 (select absolute coordinates )
N0050 U0002 (Call subroutine "U0002".... N MUST use N1234 format, U Must use U1234 format)
N0100 M30 (end of program)
U0002 (whatever subroutine) (Must be formatted U1234 and of course match the call number)

In addition, the D3 seems to prefer (or may require) that the subroutines (U****) be located last in the program. I'm going to double check that today.

Another thing... Don't leave blank lines in your code...especially more than one. it confuses the machine.

N100 (empty) = Bad


Because the D3 (and probably D1-2) allow you to use other line number formats (including cyc/sub) at the control, and allow you to send everything except cyc/sub in other line formats via serial/V24/rs232, it is very easy to get caught by this problem.
Basically it is a Grundig "bug". It converts whatever you type to a 4 digit number in it's memory (while still displaying exactly what you typed), but they forgot to make it convert cycle/sub line numbers calls (or couldn't).

************

[ 05-31-2006, 04:56 PM: Message edited by: Sean S ]

Ross, yes you are lucky to have a D4.
I think I actually do fine without most of the additions it has over the D2/3.
Two things need to be considered when talking about the differences between the D1-D11...

First, if the person is using a CAM program, and secondly, the fact that the base physical machine hasn't really changed much through the series.

Here's why...
The D4 has 256k? of ram. The Cam program I'm using easily spits out G-code close to 2MB or even higher when I'm playing with mold making type files. I realize that with DNC/drip, that the D4 could probably do these, but the base machine is not really suited for this type of work since what makes these machines so accurate and tough (rigidity) requires weight and these axes don't fly around at high speed well.
Even if they could, the spindle speed can't keep up or would be abusive to the machine constantly running at the top end and shortening its lifespan.
3D contouring at acceptable speeds/feeds would take an enormous amount of run time.

Most of the "mechanic" type files I write are in the 5K or less catagory so the 24K of the D3 works just fine.

Point is, I *do* wish I had 256K, but think it would not often get used, and even if the machine had unlimited memory (PC retrofit), the machine is a poor platform to run those files.

It would also be nice to be able to store more than one program, but in the age of CAM and RS232, it takes about 30 seconds to load a new program and I really prefer them on the PC for storage and editing anyway.
For me it is actually easier to edit the G code in a text file and re-load it to the machine than it is to key in changes at the control (Ok....a little change at the control is OK), so multiple programs seems like more of a production plus where the operator has a bunch of choices and the program lock key is on.
The 256K over the 24K seems like it would affect a small number of desired programs (if used entirely for 1 program).

Point is, when I look at it on paper, I really want the additional ram, but when I look at it compared to what I'm actually doing with the machine, and what I would like the machine to do, the D2-D3 aren't so bad and suit the physical dynamics of the machine well.

I don't think you will be unhappy with the D2 overall.

Sean

Well ,looking at the differences the additional memory is not my first concirn. Before the addition of the DNC feature i was quite happy making 3-D programs and cutting to replicate castings (sort of inverted mold work)by simply breaking down the programs into smaller programs and running them as seperate parts...worked fine. As to the time needed to preform a complex 3-D part of any size..yes it takes time baised on the spindle speed. I do not have the oiptional 6300 RPM vertial head (darn) so i am limited to 3150 (actually 3500 by real strobe test) I have run the parts needed in a "lights out" condition where i setup the machine and go home. You can do this if you have good program simulation on your CAM program and a Post you can trust to give clean no error code. I have run my machine at times for 12-14 hours non stop at max spindle speed. (i don't think it is any harder on things once the temp has reached its working range for the speed you are running.) Note i do lube my main spindles yearly.....and have seen no preciptible wear in the clearance of the spindle since i got the machine.
The areas i think that the D4 is nice is in the ease of use....the transmit/recieve/ setup of send recieve peramiters all in one spot are nice. The ability to do Macros is a real plus if you are programming on the control , and the peramiter programming is quite nice for some kinds of work.
The real advantage for me of the D4 is in its ability to helical mill..i use thread milling via single point tool all the time! I encounter so many wierd thread types in my work tht thread milling is worth the difference alone.
Also the multi program ability is also a real time saver for my application. I keep several programs in memory all the time. I do a ton of boring, both vertical and horizontal. I keep a program for each in the control all the time. When i need to bore a part i simply reset the depth values and go....
Further a real tool compensation register that is applied to all tools and does not need to be re-called for each tool is a real plus and makes fine tuning the cut size,or depth very simple.

By the way, a D4 does not use the "U" line marker for a sub routine. It uses the "x" key as in "Times" not as in the axis. Simply press the "times " key and the program drops into a new window that is only for the sub routines of that main program...Press it again and you return to the main program ..quite simple and easy.

The FP-NC's are not production machines but with a D4 control they can do a fine job of making 3-D contours if you have good software and are paitent. I know of more than one shop that is running their FP4NC's with a D4 control to make molds on a daily basis.

If i had a machine i was using on a regular basis, and it was fitted with a D2, or D3 control to me it would be worth the cost to do an upgrade to a D4...... But that is just my sense of it.


Cheers Ross

But that is just my sense of it.

Click to expand...

...and you would know better than most all of us. It sounds quite exciting.

I know of more than one shop that is running their FP4NC's with a D4 control to make molds on a daily basis.

Click to expand...

...and i believe that, but if I run a program based on machine values for say...a Haas VMC, even after stepping down the values to the max values of the FP4, I'm just not happy with how fast everything is moving. Coming into the corners and such, it's jerking the machine around. My FP4...having a toolchanger is extremely stable because of the solid 1" plate that keeps the machine and the ATC in perfect alignment, but it still moves and vibrates enough at its maximum envelope to make me feel like I shouldn't be in such a hurry.

I have run the parts needed in a "lights out" condition where i setup the machine and go home.

Click to expand...

Wow, now that takes Ba**s Ross. I'm envious of your confidence.
I cannot imagine running a part for the first time unattended.
I doubt I'll ever get to that point. I'm just too paranoid about milling through my precious table and I don't trust modern software to never glitch, let alone the 20 year old Deckel chips (and I especially don't trust that I won't make a mistake somewhere).
You are a race car driver, and I am a race car collector who likes to take it for a spin once a month. No part to me is worth potentially damaging my prize.
I really am envious of your confidence and skill tho'.

i am limited to 3150 (actually 3500 by real strobe test)

Click to expand...

...a 50/60hz thing? Have you tested any of your other speeds? It would be good to know so I could adjust my post.
You'll laugh, but I have my max spindle speed set at 2000rpm in my post processor. all feeds are based on that or lower.

Ross, you and I make good polar opposites on this board. Your skill level, usage, and collection value appreciation percentages vs my 180 degree percentages, yet we both still love the machines equally.

It's always good to hear your perspective.

Sean

..a 50/60hz thing? Have you tested any of your other speeds? It would be good to know so I could adjust my post.
You'll laugh, but I have my max spindle speed set at 2000rpm in my post processor. all feeds are based on that or lower.

Click to expand...

I think you are exactly correct! When my machine came from Germany (imported as a used machine through Ferrostal the USA dealer ) it came with the change pulleys for 60hz. I never checked the part numbers but i think the pulleys are wrong! When i conpaired them to the originals one of the pulleys was exactly the same size as the one it was to replace.......and the belt was almost too short to fit around the new setup. I had some trouble with breaking taps so i checked the speed and indeed the machine does run fast in all ranges. Never seemed like a problem so i just left it alone. Suppose i could have ordered the parts again and seen what came, but just never did. I made a table of actual speeds to use while tapping and went on with the work.

Sean: You are quite correct in things you say about the control and the machine moving. Can't compete with thoes guys running a Haas or a Hurco, but thankfully for me i don't ever have to...them guys can't do what i can with my 20 year old iron and i would not want to do what they have to do to make a living....

As to the race car thing , in our world as long as you have the cars idenity nothing else matters...they were built by men in the first place and making them again is just work, remember when everything is done it is just metal I don't consider them as disposible, however i make a good living rebuilding them and fixing what gets hurt at the track (of course it helps to be working for people that don't have to worry about where they are going to buy their next cheeseburger)

I think the ultimate FP-NC for me would be an FP4NC with the optional 2 speed vertical head, the universal table, retro fitted to have high pressure coolant and a current Heidenhain control...cures the hurkey-jerkey movement. I don't care about high speed rapids...(think most of that is sales hype as few moves ever use the speed they claim because they are too short). Add in a spindle speeder and i would be set for what i need.

Cheers Ross

And your ultimate machine, Ross, is exactly why DonS still has a job, I suspect. Although the machine might be obsolete for a lot of people, there is a contingent, such as yourself, that keep it going... and keep retrofits alive. Obviously the market isn't big enough to have tons of people in it, but it seems like Don keeps himself busy, which is good...

--Alan

That machine sounds great Ross. I'd probably go Siemens though (I just like their modular approach).

Taps...you had to say that. As I write my post, I'm getting ready to do the tapping cycle. Any advice? What sort of holder do you use? Full floating...half floating...?

Have fun modifying your post for the spindle speeder. I'm getting prepared for this one...how to do the correct code to choose the speed increaser IF the tool diameter is less than x while at the same time choosing the correct gear speed to get your speeder running at the correct speed, while at the same time keeping the correct feeds for the higher speed even though the actual spindle is programmed at a much lower speed...etc...etc. Seems like a mess. It gets worse when you consider the 4X (or other) speed multiplication and how wildly off that could be (4X the error we currently are OK with). .... sigh....

Oh, and I wasn't trying to suggest a connection between the Haas and the Deckel, and what they are capable of. I was trying to point out that I think what the Dialog controls can make the machine do are already pretty darned close to the limit of what we should ask the machine to do.


Sean