[nzben]

I have an Arrow 500 with CT controller. I have no training in CNC - jst thought I'd buy one and have a play for kicks. I'm using an old version of visual mill to process my files. Many of my circles were coming out as polygons which to me is not really what I want.

I found a setting in VM to change so it doesnt make a circle out of a bunch of lines and treats it as a circle - sweet!

However it doesnt work on my machine, it's giving an error of - end point of circle not on circumference.

the code goes something like this:

G0 X-8.732 Y-26.234 Z1.25 M08
G1 Z-0.2
G17
G3X-13.995Y-19.577I-14.691J-25.537 F150.
G1 X-14.183 Y-19.555

From what I figure - the start point of the arc is X-8.732 Y-26.234, the end point of the arc is X-13.995 Y-19.577
this is the bit where i get stuck ....
The center of the arc is -8.732+-13.995 = X-22.727
and -26.234+-25.537 = Y-51.771????

Is that pretty much it? Ill have to draw it out on some graph paper to make sense of it.

Whos wrong - visual mill, the CT controller or me? I woulda thort a computer figuring that sorta thing out should get it right - is it jst the syntax thats wrong??

[txcncman]

See attachment:

[nzben]

thx for that TXcnc, saved the graph paper, so how come visual mill cant see that? How come its giving impossible coordinates? Any good suggestions on good value cam software that can do circular interpolation?

[nzben]

thx for that TXcnc, maybe my maths was wrong?
i did a similar plot and it worked out??? where do I need to look to resolve this? VM or my machine? Perhaps its how the data is laid out?

[uli12us]

If your drawing is true, you have simply changed the I and J amounts.

[txcncman]

Most machines need I and J values to be incremental distance from the start point, which is the way I drew my example (the way your machine is reading the code). Your drawing is giving I and J as absolute coordinates. There should be a setting in your software to change the output.

[greg b]

Try putting in your cordinations and then add a (p) and what ever the radius is e.g g1 x0 y0 g3 x150 y150 P75 F200 depending on if its a non symetrical radius you may need to add a P -.Good luck

[uli12us]

@tx..; He have the I + J as incremaental values. The Zeropoint is in the upperleft corner with the two red arrows. Only I has the J value and Vice versa.

[greg b]

Sorry Man I misunderstood you,I thought you had a arrow with Acramatic A2100 control they have some different address letters on programming.

[nzben]

I thort I had drawn my I and J as incremental? My manual calculation was definitely out - but thort I had the drawing down pat?

I guess first I have to figure out where the error is, my drawing says the code is ok - tx says it's incorrect and my machine says its incorrect.

One thing I'm wondering is, VM defaults to sending 4dp output, in an attempt to speed it up I reduced it to three dp output - is it possible that the machine is seeing a rounding error due to lower resolution?

[beege]

nzben,

Cincinnati had been an oddball as far as arc definition goes. At least the controller I used 20 yrs ago. While most every other controller defined an arc using a center point relative to the arc start point (incremental), they decided to us a center point relative to the part origin (absolute). They may have switched at some time, I don't know, but you need to know which method the controller uses. Then you have to adjust the output of VM accordingly, as it might be putting out code contrary to the machine's requirement. Good luck with all that...

[nzben]

Problem solved! - sorta! Thanks for everyones input, turns out the values it needs are from the center of radius to start of arc, not from start of arc to center of radius.

However... It seems at this point my old copy of visual mill doesnt really cut the mustard and is soley using curves for engage and retract and not picking curves off the parasolid. looking in the help file I found this:

When part geometry is loaded in VisualMill, it is immediately faceted or triangulated before being displayed. This faceted model is what is used for both the display as well as the machining computations

So I guess it would never know what is circular and what isnt. Time for an upgrade me thinks. Do most CAM packages these days produce true circular paths? Is it something I need to specifically look at as a feature?

[txcncman]

I thort I had drawn my I and J as incremental? My manual calculation was definitely out - but thort I had the drawing down pat?

I guess first I have to figure out where the error is, my drawing says the code is ok - tx says it's incorrect and my machine says its incorrect.

One thing I'm wondering is, VM defaults to sending 4dp output, in an attempt to speed it up I reduced it to three dp output - is it possible that the machine is seeing a rounding error due to lower resolution?

Yes on the resolution. Most controls do error checking to 0.0001. This is usually adjustable by a machine parameter. Attached is you original code in backplot with the error forcibly ignored. Probably not the toolpath you had in mind.

[txcncman]

Problem solved! - sorta! Thanks for everyones input, turns out the values it needs are from the center of radius to start of arc, not from start of arc to center of radius.

However... It seems at this point my old copy of visual mill doesnt really cut the mustard and is soley using curves for engage and retract and not picking curves off the parasolid. looking in the help file I found this:

When part geometry is loaded in VisualMill, it is immediately faceted or triangulated before being displayed. This faceted model is what is used for both the display as well as the machining computations

So I guess it would never know what is circular and what isnt. Time for an upgrade me thinks. Do most CAM packages these days produce true circular paths? Is it something I need to specifically look at as a feature?

Most CAM software have the ability to make true arcs or arcs represented by line segments depending on software settings.