DNC Problem

[Sharab85]

I am slowly getting used to this new to me mill, a partner 3 with centurion 6 control. I have been doing programs that could fit in ram memory but recently tried my hand at DNC Drip feeding the machine through the RS232 port. Everything was going great until first tool change there it asked me for tool 3 which was the previous tool, I thought weird and just loaded the next tool, tool 5 after hitting tool change button it asked for another tool change this time for correct tool tool 5 (which is a drill). I thought great hit tool change again and it drilled first hole, well it was supposed to drill three holes total but it only drilled the one and asked for tool change again, well I was stupid and just hit tool thinking it would just drill the rest of the holes, well it didn't it moved on to next operation which was a chamfer operation so i very nicely crashed the drill chuck. So why did it skip the last two holes, i ran the gcode through a simulator and it shows drilling all the holes.

Ignore small hole in picture it is just from stock I used.

I am using fusion 360 and the generic milltronics post that is included.

I will see if I can attach gcode.

This is what I am using for DNC transfer. https://www.amazon.com/gp/product/B0...?ie=UTF8&psc=1

Thanks,

Shawn

Similar Threads:

• DNC Problem
• Problem- Dnc problem
• DNC problem
• dnc problem
• Haas Vf-2 Dnc Problem

[Sharab85]

Here is the section for the drill cycle.

(DRILL2)
M6
N17235 T5 M6
N17240 S4200 M3
N17245 G54
N17250 M7
N17255 G0 X3.3 Y-2.0625
N17260 G43 Z0.59 H5
N17265 G0 Z0.19
N17270 G98 G73 X3.3 Y-2.0625 Z-0.9627 R-0.11 Q0.562 F40
N17275 X4.05 Y-1.3125
N17280 X3.3 Y-0.5625
N17285 G80
N17290 Z0.59
N17295 M9

[Brian L]

Looks pretty normal (the code), except you don't usually see to many R minus values in the drill cycle unless you are drilling a surface lower than Z0 and there better be nothing in the way as you move from hole to hole.

That said, I've had instances where DNC gets corrupted code and doesn't run right. Take a look at your baud rate and such and see if that changes anything. Also, always best to run the whole program a couple inches high the first time thru to verify things are working correctly... saves on drill chucks, tools and fixtures. I don't see that part having enough code to need to use DNC, looks pretty simple to me.

[machinehop5]

,,,that extra M6 may be causing problems.

quote:
(DRILL2)
M6
N17235 T5 M6
N17240 S4200 M3
N17245 G54
N17250 M7
N17255 G0 X3.3 Y-2.0625
N17260 G43 Z0.59 H5
N17265 G0 Z0.19
N17270 G98 G73 X3.3 Y-2.0625 Z-0.9627 R-0.11 Q0.562 F40
N17275 X4.05 Y-1.3125
N17280 X3.3 Y-0.5625
N17285 G80
N17290 Z0.59
N17295 M9
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF)
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING)
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID)
(MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)
(2D CHAMFER1)
M6
N17300 T4 M6

good luck hunting

[Sharab85]

Ya the drill cycle is after some adaptive clearing that reduced the z height to start the drilling. The program is 100kb and my parts storage is a little over 150kb but I almost crashed system by trying to load it into memory without deleting other programs. The control would not boot up properly a couple times to let me delete stuff. I figured I better get used to dnc operations if I want to do anything remotely complex. I am wondering If it could have anything with running it dnc fast vs run.

[Brian L]

Good catch on the double M6 call outs, not sure that is the issue though. I tend to run only one program in the machine at a time, don't store anything there. Load it, run it, download it with any changes made back to the PC and that way nothing is clogging up the memory.

I only used DNC a few times and it was always DNC Fast, but if I remember correctly, that was only single tool huge 3D programs, several mb in size. Fusion is terrible for writing huge bloated programs that no older machinery can run because of memory size, I know there are settings in Fusion that will help, my son uses it, but I use a simpler, less "useless code" software called Sheetcam, it's pretty archaic, but for simple 2 1/2D parts it's a whole lot lest code.

I got tired of the whole mess and retrofitted the machine with a Centroid control with no limits on program size.

[Sharab85]

Well figure out one problem find another. It turns out that it is the DNC fast that is skipping the drill cycle, I ran it DNC run and loaded it into memory and they they both run cycle fine but DNC fast still just drills first hole and then just positions over other holes and finishes program.

Great I will just run programs DNC run BUT during DNC run on one of the arks will act very jerky like it is trying to stop at every point along the way, it will not do this on DNC fast or if loaded into memory. It only does this on two arks around the N2100 line. It will even be very jerky when I turn the feed way down.

[Brian L]

You would have to look at the code, but Fusion will sometimes write an arc using hundreds if not thousands of little tiny .001 or so straight line moves instead of one G02/03 line of code. If that is the case, the older Milltronics processor can read lines of code that fast. Again, Fusion has settings, I think in the posting dialogue that will force G02/03 code instead of many small segments of G01.

[Sharab85]

Ya I figured it was something like that it is just weird that it is doing it on only DNC run and not with DNC fast for reading from memory.

[Brian L]

DNC fast is just that, it reads the lines of code much faster, which is what you run into on a lot of 3D parts.

[machinehop5]

...few more things that we need to know/check:


What PC software is being used to DNC to CNC?

How is the Cable wired? How many wires,,,Is it homemade?

Are you using XON/XOFF for Flow Control?

Do you have a detailed G Code List for your CenMilltronics Ver6 you can post or link to?

[sportybob]

Well figure out one problem find another. It turns out that it is the DNC fast that is skipping the drill cycle, I ran it DNC run and loaded it into memory and they they both run cycle fine but DNC fast still just drills first hole and then just positions over other holes and finishes program.

Great I will just run programs DNC run BUT during DNC run on one of the arks will act very jerky like it is trying to stop at every point along the way, it will not do this on DNC fast or if loaded into memory. It only does this on two arks around the N2100 line. It will even be very jerky when I turn the feed way down.

Hi Sharab85, If you are DNC'ing form a floppy , That could explain the pause and dwells,( read times from a floppy are "slow" ) the other thing is possibly the post processor, trying to do an arc with a "bazillion: little line moves. Turn the "arc filters" on on your cad/cam. This will take an arc move from "a bazillion moves" to a single IJ move.
In standard DNC you can watch the graphics, in DNC fast, (no graphics), larger programs can be loaded to the RAM drive and run from there.

The other suggestions from other Milltro users as valid as well, how is the cable, how is the RS-232 set up.?? etc:


Sportybob