What's new
What's new

Capabilities Dialog 2 to Dialog 3/Thread milling

Martin P

Titanium
Joined
Aug 12, 2004
Location
Germany in the middle towards the left
The subject had come up in a conversation which Dialog control can do thread milling.

I have now come across a Deckel operator manual from 1985 (the month is not legible) called:

CNC control Dialog 2 and 3
Graghics
Contour Pocket
Thread Milling
3 spindle head
NC- dividing head
Upgrade package

Its in german, but is also very misleading in german.

From the title one might think that Dialog 2 can now thread mill. But in the introduction it says:

“In this manual you find
-the standard extensions of the Dialog 3 as compared to the Dialog 2
- the extensions, which are offered as options for the Dialog 3”

What is an option and what not is not said outright, but in the manual in then identifies graphics and Contour pocket as an option.
So in conclusion one may think that at least in 1985 the Dialog 3 had thread milling and the Dialog 2 did not.
By extension one may surmise that D4 always had thread milling standard.

I seem to recall an upgrade to the D2 for thread milling, but this may never have happened.

The title seems to indicate a separate “upgrade package”, but that is just very bad writing, as this IS the package.

The Deckel literature always and consistently seemed to want to keep the customer in the dark on some subjects. I am sure many customers bought a machine only to then find out that the sales brochure capabilities were not included. All D4 sales brochures mention graphics, but they rarely clearly mention its an option.
 
My d2 manual says no thread milling.
I have a d3 manual it may or may not be optional. the back of the manual after troubleshooting and accessories has thread milling
I have a supplemental manual d2/d3 (2of 1985) says you could upgrade d2 do thread milling contour pockets and graphics. I guess it make it a d3 with optional upgrade package.
check with DD for more specifics.
Dave
 
One must be careful here.
To me there are two distinct types of thread milling...
There is the factory G77, G78 thread milling that i believe what the above posting is talking about.....

Perhaps a bit off the original topic but of interest to me:
There is another form of thread milling that i use that is of interest to the prototype worker.
That would be the ability to "single point" threads with a milling cycle.
My late software version D-4 does this, but not, to the best of my knowledge, my early (no NEP 52) home D4 flip FP3NC.....

What is required to do single point thread milling is the ability to program a circular move in polar coordinates...ie G9 and that move must allow a depth move as part of the G9 call.....
or "helical milling"

The good thing about this method is that it allows use of simple cheap tooling...I run a standard ID thread turning bar gripped in a collet ...interpolate the major diameter while moving the pitch in depth.....
Allows long threads to be milled and literally any diameter or pitch that the math can solve.....

Think if your machine can do a G02 G03 move and the control prompts for a depth value (or not) you can do single point thread milling....If not then you can't.....Not sure if this is a software or hardware requirement, but it is not possible on my early D-4,(at least i haven't figured out how to do it yet) so i would guess it is not an option on a D-3.....

Cheers Ross
 
As usual I am not an authority on this subject.But I'm learning more everyday about NC Deckels and Dialog controls.From what I gather when D2 came out it could not thread mill but could with later software and I assume for all intents and purposes could be upgraded to a D3.When D3 came out it could thread mill ,however I'm not sure if it was an option or not and if so, if it was a pay for flip the dip switch option?To me all this bullshit about options is ridiculous:icon_bs:.If it's in the machine let it be used.This jive is still pulled today apparently only with passwords:rolleyes5:.
Ross,
I've never thread milled before but I'm fixin on it.
I assumed all thread milling had the same dynamics and I thought the specific pitch tools were for higher production.
The way I see it two axis are interpolating the od or id and the third is running the pitch rather it's single or multi point.
Is the difference being that a single point tool would be less ridged and not as fast cutting with only one point thus requiring different parameters or what not.Multiple passes, higher spindle speed and slower feed?
What am I missing?
Regards, Mike
 
Mike:
You are correct.....
The thread milling cycle on the Dialog control is a canned cycle and it only allows one revolution of the tool on the ID or OD of the part.
The depth move only makes one pitch advance in that single turn....
With this cycle you must have a cutting tool with multi teeth and long enough to make the full length of thread at one time.....
This makes the production of threads pretty fast as you are only moving the tool into the hole, then arc into the depth required and interpolate one revolution while feeding in or out (right hand or left) one pitch, then arc out and return to the tool change point or position for the next thread.

Although faster, there is some trade off in surface finish i think as you have a cutting edge in every thread in its full depth. Also the length of thread that can be milled is limited as are the number of pitches...(got to have a cutter/insert for every pitch you want to cut).

The method i described in my earlier post is really an extended helical milling operation...
Here you use the single edge thread tool, or a multi edge cutter that has a single pitch....(small double angle cuter on a stick)

Here you program the degrees of rotation (on the dialog 4 you can use up to 9999.9999 degrees in a polar move)based on the depth you want the thread and advance in depth to match the pitch you are trying to cut.

Advantage here is that you can cut any pitch you wish and almost any length ...it does require multi passes usually, but the finish is generally better than the multi tooth thread mill setup. \

For a home shop guy the single point ability is nice as it cuts expensive tooling costs...at the loss of through put.
For me it allows making non standard threads for fitting up repair sleeves in worn bearing housings etc.....

It also allows matching an existing thread by using the movement of the quill to correct position of the cutting tool in the groove...
The single point method further allows seeing the thread as it is being made before the entire depth is reached for a full length as with the multi tooth tool....
Finally, i think that the single point method might have some advantage in threading hardened materials....

Cheers Ross
 
Ross,
Now I'm kind of disappointed.I either overlooked the listed limited capabilities of the Dialog thread cycle or was misinformed by deckel literature.Maybe I'm expecting too much from such a dated control but I just assumed "thread milling" meant full on.I'm still in infantile stages of programing but couldn't one omit the canned cycle and program a dialog 3 or 4 to get real thread milling results(desired length/depth and pitch)? Or is that what your already describing?

Regards,Mike
 
The upgrade booklet I refer to from 1985 is confusing even in my native language, but it appears to describe 2 methods.

1) D3: mill a thread using G02/G03 with a defined advance like Z or Y. This will only work up to 1 revolution and for more revolutions one has to program accordingly more.

2) D3: G77/G78 cycle, which considers pitch and thread number. I see no maximum number of threads mentioned.

3) D4: The SW upgrade package manual for the D4 from 8.87 also mentions the programming of a screw line. In this manual its treated like a new thing that the control can also move in Z when doing a G02/G03. Yet it is the same as no. 1), only 2 years later.

4) D4: upgrade manual: "programming a screw line using G9 G2/G3". This is milling a thread using polar coordinates and can be used up to 100 thread revolutions.

One may conclude from this data that an early D4 had less capabilities in thread cutting then a D3 (no Z when using G2/3). But it certainly had the G77/G78 cycle. Look at the D4 introduction leaflet from 1985 mentioning thread milling: Dialog 1 to 4 + Cont. 1-3 - Deckel NC Milling Machine Web Site

If Ross can not thread mill using any of these methods using an early D4 I would think of a defect.

Martin
 
Ross is right,
the g77/78 cycle only does one helical move. It is really nice if you are threading a lot of holes, as they get done quickly.
I use Martins # 1 method and a single point tool for smaller # of holes.
Dave
 
In case anyone isn't familiar with the single point thread milling that Ross has described here's a short video of single-point threadmilling 3/4-NPT in a plastic part. Sorry about the lighting, I should have turned off the Waldmann light on the machine.

(The machine isn't a Deckel though it's sorta related as Hurco made some controls for Deckels.)
This was programmed in Hurco's conversational. I'd think that any machine that can do helical interpolation could single point threadmill.

I use this technique often as the prototypes that I make have a variety of different threads. To have every threadmill on hand would get too expensive.
 
I have used D4 to single-point taper pipe threads. I computed the mathematical best-fit arc to each quarter turn, with the constraint that the start point of each arc had to coincide with the end point of the prior arc, and that the arcs had to be tangent at each junction. The arc radii and pole locations are the parameters computed from the fit. I can provide more info when I get back from this business trip. The resulting thread is way better than any die could produce.
 
The upgrade booklet I refer to from 1985 is confusing even in my native language, but it appears to describe 2 methods.

1) D3: mill a thread using G02/G03 with a defined advance like Z or Y. This will only work up to 1 revolution and for more revolutions one has to program accordingly more.
Martin,
So in other words it should be possible to single point thread mill with a D3?

I have some rather large nuts I need to make and I'd rather not do them in a lathe.
 
Martin,
So in other words it should be possible to single point thread mill with a D3?

I have some rather large nuts I need to make and I'd rather not do them in a lathe.

I do not think so.......Single revolution with one pitch advance in depth.
If someone out there has done "real" single point on a D3 i would love to hear from them.....

The question that remains: "is will a D3 do real helical milling, or more to the point a real polar circular move with a depth componnet.".....If not then you can't single point thread mill. A G2/G3 will only make one revolution, so no single point thread unless you repeat the circle at each thread (pitch)

Believe what the booklet is talking about is doing a thread mill using a multi tooth cutter and if you need more length you advance the starting depth some module of the thread pitch and re run the thread milling cycle....Of course any errors in the exact position of the second start will be seen as threads that have an inaccurate pitch, and an undersized pitch diameter where the two cycles overlap...

Suppose you could run a thread milling cycle for each thread you wanted to cut....ie if your nuts needed 1" long thread at 8TPI...you could i suppose cut 8 complete thread cycles at .125" depth incriments......

cheers Ross
 
If the control will interpolate in 2 axis and simultaneously do a linear move in the third you can thread mill without limit. You just have to write the code :). In fact with modern CAM software you can produce an acceptable thread even if the control will do only linear moves, but the program will be big (lots of little segments).

My HH controls do not have canned thread mill cycles as they expected any hardware they were fitted to would surely have rigid tapping capability! (The HH has the ability to write custom cycles, but I have not tried that). However I wrote a post processor for OneCNC to create the paths using quarter arc helical moves as Rich describes. The math was done by the HH control because OneCNC does not allow math in the post processor. This was made obsolete by the latest version of OneCNC which will automatically generate code for thread milling on any machine, using helical moves if available or linear moves if not.
 
Problem with the Dialog controls using many small moves (CAM) to generate a single point thread cut path is the processing speed, that coupled with the lac of look ahead you tend to get notchy cuts....
Using G64 to blend moves helps but it is still an issue if running off point to point moves....That and the cutting times become huge as the control can't keep up with a reasonable feed rate....
Cheers Ross
 
If your d3 will take a z move in the g2/g3 input with your x, y, i, and j and do the helical move it will single point thread mill as deep as you want to go excluding tool limitations.
Dave
 
And now for the final confusion ...

Deckel publication "Die neue CNC Dialogsteuerung 2" (the new Dialogcontrol 2) from April 1983 (!!!), technical status from April 1983, printed in July 1983.

Page 17 shows this:

Dialog2ScrewLine.jpg


Text: screwline interpolation: the simultaneous control of 2 axis circular and 1 axis constant feed makes the milling of screwlines possible.

BUT, in back of brochure in the specs pages, this capability is not mentioned.

I tried to use this function yesterday in the Deckel desktop programming station (upgraded to Dialog 3), but I could not make it work. Also the attached reference manual did not mention it.

BUT the Dialog 2 brochure shows the typical Deckel standard part WITH the helical interpolation. The Dialog 1 brochure is just blank there.
DeckelStandardPart.jpg



Soooo, what does this mean? Several possibilities come to mind:
1) Deckel did not know what was going on. Promises made, customers pissed.
2) Some capabilities were options, and not so identified.
3) We are all too stupid to use this function.

In my experience incompetence is always the by far most likely explanation for anything, in this case on the Deckel corporate side. There is a reason they went broke. Marketing just made brochures, no matter how Grundig kept up. Its the german version of Dilbert.
Of course the question is still open of what control could do what from when on.
I am pretty sure that if you went to Deckel in 1990 to get helical interpolation on a D2 they would sell it to you. Probably without having to by the D4 upgrade (which was like buying a new control).
 
No Ross I don't have one now,
I Did have a new fp4nc in 1984, 85 d3 3150 non flip head and it had the optional upgrade package and would do contour pocket, thread milling cycles g77,78 and helical like the d4. Will your d3 do contour pockets and g77,g78 if not it probably doesn't have the upgrade.
If the d1 or d2 had fourth axis capabilities yes you could thread mill but only on center of rotation. My 3m will do helical but has no thread milling cycles. I guess I could write a parameter program to make a single point thread milling cycle or do the same on the d4.
If the need ever arises I will make time to do it.
Dave
 








 
Back
Top