What's new
What's new

Deckel FP2NC Dialog4 Helix

artelogic

Plastic
Joined
Oct 9, 2020
My FP2NC shortly pauses after each G2/3 with X,Y,Z as it was in G60-Mode, although it is in G64-Mode. Is that normal?
G2/3 with X&Y only it runs smooth as expected.
 
My FP2NC D4 does smooth helixes (helices?) within G41...G60 M61 //// G40... I use G09 polar coordinates. My machine has the latest software update that was available, although I forget the number... 3.7 maybe? What is your feed rate? Can you post a code sample?
 
N10 G53
N12 G90
N14 G64
N16 M62
N18 G17
N20 M9 M5
N22 T1
N24 S+800 F80
N26 G0 X-1.643 Y-5.461 Z5
N28 G0 Z1.125
N30 G1 Z-1.625 F80
N32 G1 X-0.276 Y-4.001
N34 G3 X-1.643 Y-3.461 I-1.367 J-1.46
N36 G3 X-3.103 Y-4.095 I0 J-2
N38 G3 X-3.22 Y-4.225 Z-1.681 I3.103 J-2.903
N40 G3 X-3.331 Y-4.359 Z-1.736 I3.22 J-2.773
N42 G3 X-3.436 Y-4.497 Z-1.791 I3.331 J-2.639
N44 G3 X-3.534 Y-4.639 Z-1.844 I3.436 J-2.501
N46 G3 X-3.627 Y-4.784 Z-1.897 I3.534 J-2.359
N48 G3 X-3.714 Y-4.932 Z-1.949 I3.627 J-2.214
N50 G3 X-3.794 Y-5.084 Z-1.999 I3.714 J-2.066
N52 G3 X-3.869 Y-5.24 Z-2.048 I3.794 J-1.914
N54 G3 X-3.892 Y-5.292 Z-2.064 I3.869 J-1.758
N56 G3 X-3.956 Y-5.448 Z-2.108 I3.892 J-1.706
N58 G3 X-4.014 Y-5.604 Z-2.15 I3.956 J-1.55
N60 G3 X-4.066 Y-5.763 Z-2.19 I4.014 J-1.394

The first two G3s (N34+N36) run smooth, the following do not.
 
I don't think your G64 and M62 are doing anything. They are meant to be used within G41 and G42 tool radius compensation. Here is code for a 10-turn internal thread helix with a 2.772-mm radius and 0.5 mm lead (M5.5x.5) using the horizontal spindle. The tool starts down in the hole and spirals out counterclockwise. The entire helix is coded at N190.
...
N120 G18 T2
N130 S+3150
N140 G0 X0 Y3 Z0
N150 Y2 F60
N160 Y-11 F75 M70
N170 F125 M70
N180 G41 G46 A1 X2.772 Z0 G1 G60 M61
N190 G9 G3 M71 W3600 G90 I0 K0 Y-6
N200 G40 G46 A1
...

I am not surprised the ancient control pauses because it cannot keep up with the number of steps in your code. Use G41/G40 and G9 G3 (G2 for external thread, assuming climb milling) and life will be much better.
 
Probably stalling the old D4 control, as already mentioned.
Even Dialog11 can be stalled, if you try hard enough (I know) ;-)
Your G-code is some weird spiral, if I simulate it?

Thread milling works very well for me on my D4 with Software V2.32, but I do it in a single line with polar coordinates.
 
Yes, it is to chamfer are 3D-Spline. But it is not the complete code, it's even longer.
Screenshot_20211024_123535.jpg

But the the G64 does something. If I use G60 instead with a simpler geometry, it pauses after each line.
 
The thread title word "Helix" threw me off. Now I see what you are trying to do, and I don't think there is a way to avoid the pauses. I have run into the same issue trying to cut a similar saddle shape. You can minimize the pauses by using a CAM program, turning on "smoothing" (which fits arcs to the path), and putting a big tolerance on the fitting between the arcs and the actual tool path in the design.

I can't tell you why G64 does anything outside of a G41/G40 compensated path. I don't think it's documented in the manual.
 
I can't tell you why G64 does anything outside of a G41/G40 compensated path. I don't think it's documented in the manual.
I asked about G64 and didn't get an answer here. It's not documented well in my manual either. It does work outside of G41. I found that the G40 turned G64 off, and I had to put G64 on the next line if I wanted it to continue to be effective. When cutting a series of small arcs or line segments, G64 made it smoother and prevented the stops at the end of each segment even when cutter comp was not active.

Having said that, I don't see anything in the OPs code that would turn it off. Do you still see G64 on the monitor while it is pausing? If you switch to distance-to-go mode do you see zeros on the screen for all 3 axes at the pause? If you turn the speed override way down to give the control more time to process does it still pause?
 
I agree with John...
Believe that the G64 does work on code even when not using G41-42.....
My post for SurfCam always calls G64 and it never uses the control cutter comp,
CAM calculates the cutter offset within the program...code produced runs smoother and with less herk-jerk if i have the G64 in force....At least that is my experience.
Never had any issues with it cancelling as the CAM does not use G40....

Cheers Ross
 
I asked about G64 and didn't get an answer here. It's not documented well in my manual either. It does work outside of G41. I found that the G40 turned G64 off, and I had to put G64 on the next line if I wanted it to continue to be effective. When cutting a series of small arcs or line segments, G64 made it smoother and prevented the stops at the end of each segment even when cutter comp was not active.

Having said that, I don't see anything in the OPs code that would turn it off. Do you still see G64 on the monitor while it is pausing? If you switch to distance-to-go mode do you see zeros on the screen for all 3 axes at the pause? If you turn the speed override way down to give the control more time to process does it still pause?

Will check that tomorrow. But I assume, the answer to my question is "yes it's normal, because the CPU is to slow".

And yes, Gs are not modal. Omitted G is interpreted as G01.
 
Well at least you don't have to load the exe. with paper tape....
And G1 might easily be seen as "modal' in that any move not otherwise defined is understood to be a G1....
Cheers Ross
 
Well at least you don't have to load the exe. with paper tape....
And G1 might easily be seen as "modal' in that any move not otherwise defined is understood to be a G1....
Cheers Ross

I don't view it as more complex, just different. In the modal, case, things get complex real fast if you forget to turn off modes like G0 or G81. Dialog is 35-year-old CNC, too.

Tell him it makes plenty of sense when programming at the console, which is what the control is optimized for.
 
Yep, and makes a nice companion to the "Lear" 8-track ya got under yer dash.....

By the way, the Dialog controls (1-4) don't loose the executive,even is the batteries go dead and you never have to load it...
Entire operating system is on E-Proms....
Control fires up instantaneously, having no boot up, she is ready to run as soon as you push the start button....
Cheers Ross
 








 
Back
Top