Need Help!- Controller not machining same as simulator

[Mike4703]

I have been programming circular pockets manually and by using "Machinists Toolbox" utilities. When I run the code in NCPlot the circles turn out the right size and in the right place. When I run the same code on my controller, the circles turn out larger (about 4 times) and dislplaced to the left. I did not get any documentation with my controller (Chinese). It is obviously interpreting the G2/G3 command parameters differently. What would cause it to come out this way on the machine despite being ok in NCPlot? I am in the process of getting support from the manufacturer but they only answer questions one at a time, sometimes incomprehensively in Chinglish, and don't seem to have a written guide to their controllers G code interpreter.They mean well but so far have not been able to give me a helpful answer on this. I don't have any problem with linear interpolation

[angelw]

Originally Posted by Mike4703 I have been programming circular pockets manually and by using "Machinists Toolbox" utilities. When I run the code in NCPlot the circles turn out the right size and in the right place. When I run the same code on my controller, the circles turn out larger (about 4 times) and dislplaced to the left. I did not get any documentation with my controller (Chinese). It is obviously interpreting the G2/G3 command parameters differently. What would cause it to come out this way on the machine despite being ok in NCPlot? I am in the process of getting support from the manufacturer but they only answer questions one at a time, sometimes incomprehensively in Chinglish, and don't seem to have a written guide to their controllers G code interpreter.They mean well but so far have not been able to give me a helpful answer on this. I don't have any problem with linear interpolation

Post a copy of your CNC program, a sketch of the drawing detail and the make and model of the control.

Regards,

Bill

[varga]

try this, with the spindle on and at the desired depth give it a g13 (climb) or g12 (conventional) it works with haas and alot of various newer controls

Ex:

G0 X0. Y0.(CENTER OF HOLE TO BE POCKETED)
G43 H1 Z.1
G1 Z-.25 F10.
G13 I.1 K1.0 Q.2 F10. D01
G0 Z2.

G13= CCW POCKET(CLIMB MILL)
I= INITIAL ARC RADIUS
K= FINISHED ARC RADIUS - 1/2 DIAMETER OF CUTTER
Q=STEP OVER AMMOUNT
F= FEED RATE
D01= DIAMETER COMP OF TOOL #1

WITH A .5" ENDMILL THIS SHOULD GIVE YOU A 2.5" HOLE
IT IS WORTH A SHOT... LET ME KNOW IF IT WORKS FOR YOU

[fordav11]

I would wait for the OP to reply with his control model first.
I *certainly* wouldn't be issuing any unknown/non-standard G codes like G12/G13 'at the desired depth' in Z minus without first testing it 6" above the part

[Mike4703]

Sorry guys, its been pointed out that I need to give the code, screen shots, and info about the controller. That's going to take me a little longer as I have been really busy these last couple of days, but I will post that info soon. Thanks for the replies so far.
This controller is made by Rich NC of Beijing China. the model is 0501. I'm almost certain it will not do G12/13. It's very conventional, doesn't do subroutines. I post more info later.

[sinha_nsit]

Even if you have some standard control such as Fanuc, the third-party simulators such as NCPlot may not show the exact behavior of the machine because so many things are parameter dependent, which these simulators may not consider. For example, G00 may or may not have straight-line path. Simulators would typically show only straight-line movement. Exact toolpath can only be seen on the graphic screen of the machine. That also assumes that G54 etc are correctly set.

[Mike4703]

Ok - The situation is that I built my own machine from a Sherline Cnc mill with Gecko drivers and RNCZ-0501 controller from RichNC. This is a pendent style controller with an interface board. I didn't want a computer in my small outdoor shop and thought it would be a good idea to program on my nice Windows 7 laptop inside and load the code into a flash drive and run it on the controller outside. Also did not like all the seventies looking software that only ran on XP. Most American or European pendant controllers that could run code were way too expensive. Now I see things a little differently. I have been unable to get any comprehensible documentation on how this controller interprets G code. Setup has been a trial and error process. That said many programs run just fine. The current size problem has been really difficult -- I have ended up finding that I need to divide the G-code parameters by 2.5 to create the desired part on the machine. This only happens when programming complete circular motion. Linear moves are made just as programmed. Attached are screen shots of a 16mm counter bore I programmed in NCPlot. Note the X value which is the radius. The machine actually makes a 16mm diameter hole with a 3.175mm diameter end mill.
(16MM CIRCLE WITH .125IN END MILL)
G00 X0Y0
G00 Z5.0
G01 X-3.20625
G01 Z-.50
G02 I3.20625J0
G01 X-3.20625
G01 Z-1.0
G02 I3.20625J0
G01 X-3.20625
G01 Z-1.5
G02 I3.20625J0
G01 X-3.20625
G01 Z-1.75
G02 I3.20625J0

Any ideas? Is it me or the machine? Or are there too many possibilities to know for sure as some of the replies here imply? I may end up buying another interface board, getting Mach3 and an old laptop but I sure wish I could make this work. I thought I was done with the electronics!

[fordav11]

the normal programming method is to use G41/G42 cutter diameter compensation which you're not using?
also normally a G02/G03 will have X Y end point as well as I and J (or R)
on a real control X Y can be omitted and it will cut a full circle but that might be confusing your toy controller

to cut a 16mm hole on a standard CNC control you would do something like this.....

G0 X0 Y0
G0 G43 Z5.0 H1 (H1 is the tool length offset)
G1 Z-0.5 F50.0
G1 G42 X-8.0 D1 (D1 is set to cutter radius i.e. 1.5875)
G2 X-8.0 Y0 I8.0 J0
etc

[Mike4703]

I'm not using cutter radius compensation because I get a "unknown character" error when I try it. Supposedly this controller can do it, I'll send another email to NCRich as see it I can understand the reply. According to the specs this controller can interpret "most Fanuc postprocessing" But for now I had to change the Gcode to:

G0 X0 Y0
G0 Z10.0
G1 Z-0.5 F50.0
G1 X-8.0
G2 X-8.0 Y0 I8.0 J0

The tool should have started at 0,0, gone straight left to X-8, and then cut a 16 mm circle measuring to the tool center since CRC is off now. See the attached picture for what happens. Disregard the two "craters" these are old tests on this piece of scrap aluminum. As you can see the linear move is 8mm but the circle is 32mm or would have been if I let it complete. It was headed for the vice jaw. The diameter is 2x off now but the center is where it should have been if the circle had turned out like it was supposed to.

[angelw]

Originally Posted by Mike4703 The diameter is 2x off now but the center is where it should have been if the circle had turned out like it was supposed to.

The centre is also incorrect relevant to the code example you included. The centre of the circle described by the I and J value should be where the White cross is shown in the attached picture. The Red cross shows the centre of the actual circle being cut. It seems that the I value, and probably the J value as well, has been multiplied by 2. 2 X J0 would still be zero, hence the reason I suspect, that the Y centre appears correct. It would be interesting to program a complete circle with the cutter starting the circular path at say, 10 o'clock, so that both I and J had a value other than zero. I would expect the circle centre in both X and Y to be incorrect.



I note in one of your earlier post that you state that this problem only happens when a complete circular path is programmed. Does it not happen when only a sector of a circle is programmed?

Regards,

Bill

[neilw20]

Machine control is set to incremental arc centers.
Put a G90.1 (absolute IJ) at the start of the program.
Your control was set to incremental IJ to machine as it did.

If you turn off absolute arc centers in NCPlot, it displays the same you machined.
NCPLot does not seem to understand G90.1, G901.1 and maybe your controller doesn't either. You may be forced to program in relative mode!!?? YUK.

Why did you get a half circle? Machine limit, or gave up.

G90.1 (absolute IJ mode)
G91.1 (relative IJ mode)
G90 (absolute distance mode)
G91 (relative distance mode)

This should work, and hopefully the center is where you want it.

(16MM CIRCLE WITH .125IN END MILL)
(RELATIVE IJ MODE, helical interpolation not so hard on the cutter.
G00 X0Y0
G00 Z5.0
G01 X-6.4125 F100
G01 Z0
G02 Z-0.5I6.4125J0
G02 Z-1.0 I6.4125J0
G02 Z-1.5 I6.4125J0
G02 Z-1.75 I6.4125J0
G02 I6.4125J0
G0 X0 Y0 Z5

[Mike4703]

Nielw-thanks, a light bulb just lit up. When I programmed a rectangular cut with radius corners previously, it worked fine, and now I remember, I did it with incremental programming. I will try your code later this week and post how it went. And retry NCPlot with absolute centers turned off. No time now until Friday morning unfortunately.

Angelw- yes, that's correct the center is off also. I aborted the cut because the large radius that was forming would have run the tool into the vise. I only had enough room if it was the right size Like Nielw observed, this may be a relative vs absolute thing. I was never sure how my controller interpreted G2/G3 parameters.