Wincnc arc question

[Eric Mims]

Got a Wincnc error today. When I load a very simple file it says Error: Arc radius. here is the whole file, just a .25" bit cutting .75" by using a helix motion. In .125 material.

my arc settings in the wincnc.ini file are g2mmodal=1, and .01 for the other setting. I tried raising and lowering it but it didn't seem to help.

------------------------------------------

G90
T1
S12000
G0 Z0.1250
G0 X0.0447 Y-0.1167
G1 X0.0447 Y-0.1167 Z0.1000 F40.
G3 X0.0000 Y0.0000 I-0.1115 J0.0509
G0 Z0.1250
G0 X0.0000 Y0.0000
M5
G53 Z
X0Y0

[Joey Jarrard]

I do not think it is wincnc can you tell me what you used to draw it. it looks like there might be a setting in the design software.

[Eric Mims]

simple circle in Rhino, toolpath in Rhinocam. I can edit the post anywhich way I want in Rhinocam, and right now I am using the Wincnc post that Mecsoft sent me.

[Joey Jarrard]

do you have this or can you save this in dxf and i will load it in to vetric and compare codes to see what we might need to change in the post

thanks

[Eric Mims]

well, there's nothing to it.. I mean, just make a .75" diameter circle at 0,0 and that's it. Extremely simple. The toolpathing I was using is called "hole pocketing' and it spirals down in a helix to pocket out holes. Above is what came out in the code.

[james mcgrew]

eric i think joey is looking for the ability to duplicate from the dxf to check the post proccessor. i'll run it today. the file looks fine it may be the pp, with the dxf we could read the difference (if any) in the pp

jim

[Eric Mims]

I know, it just wouldn't make any sense to send a dxf... I made a circle in Rhino and without leaving Rhino, used Rhinocam to make the toolpath. To convert it to a DXF and export wouldn't really help anything. I need to find out if the post processor needs to be set up slightly different for this type of function. Maybe Joey can forward the code above to Wincnc and they can say why the error is coming back and how to solve it, either in the PP or the wincnc.ini.

eric

[GJMATHEWS]

Eric, I just simulated your 3/4 in circle in Rhino and generated code for it using a 1/4 inch end mill to a depth of -.10.

This is my code for that file.

Simulation executes perfecty.

G00 X0. Y0. Z1
T2
S4583
M3
X-0.0006 Y0.1242 Z0.125
G01 Z0.025 F7
X0.0254 Y0.1224 Z0.0084 F4
X0.0575 Y0.111 Z-0.0133
X0.0853 Y0.0914 Z-0.035
X0.1068 Y0.0649 Z-0.0567
X0.1204 Y0.0337 Z-0.0783
X0.125 Y0. Z-0.1
X0.1128 Y-0.0651
X0.0677 Y-0.1173
X0. Y-0.1406
X-0.0729 Y-0.1263
X-0.1308 Y-0.0755
X-0.1563 Y0.
X-0.1398 Y0.0807
X-0.0833 Y0.1443
X0. Y0.1719
X0.0885 Y0.1534
X0.1579 Y0.0911
X0.1875 Y0.
X0.173 Y-0.0833
X0.1225 Y-0.1536
X0.0447 Y-0.1959
X-0.0457 Y-0.2002
X-0.1308 Y-0.164
X-0.1931 Y-0.093
X-0.2188 Y0.
X-0.2011 Y0.0968
X-0.142 Y0.178
X-0.0517 Y0.2263
X0.0526 Y0.2307
X0.1503 Y0.1885
X0.2212 Y0.1065
X0.25 Y0.
X0.2023 Y-0.1469
X0.0773 Y-0.2378
X-0.0773
X-0.2023 Y-0.1469
X-0.25 Y0.
X-0.2023 Y0.1469
X-0.0773 Y0.2378
X0.0773
X0.2023 Y0.1469
X0.25 Y0.
X0.
G00 Z0.125
G80
G00 X0 Y0
M05

Keep in mind, I am not using the preset ini files from WinCnc to cut circles arcs or to do hole pocketing. This is the way my post processor is setup. The file may seem a little long, however, I get crisp pocket holes and perfect circles.

To be honest, the way your code is generated is the first time I have ever seen it with an I or a J. Just goes to show you there is more then one way to skin a cat in G-code.

[Eric Mims]

Interesting.. thanks Guy, when you find a second, could you possibly email me whichever post processor file you used to create the toolpath. I think they are .spm files in the posts directory. I can compare it to how mine is set-up.

Thanks!

Eric

[GJMATHEWS]

You got it.

[Eric Mims]

this is what I got by using that PP:

G00 X0. Y0. Z0.
M06 T1 S4583 M3 X-0.125 Y0.0001 Z0.125
G01 Z0.025 F7
G17 G03X0.125Y0.Z-0.1I0.125J-0.0001K0.25 F4
X0.25I-0.125J0.Q0.0625
X-0.25 I-0.25 J0.
X0.25 I0.25 J0.
X0. I-0.125 J0.
G00 Z0.125
G80G00 X0 Y0M05

I'll look deeper into it tonight when I get some more time

[pescado_loco]

Got a Wincnc error today. When I load a very simple file it says Error: Arc radius. here is the whole file, just a .25" bit cutting .75" by using a helix motion. In .125 material.

my arc settings in the wincnc.ini file are g2mmodal=1, and .01 for the other setting. I tried raising and lowering it but it didn't seem to help.

------------------------------------------

G90
T1
S12000
G0 Z0.1250
G0 X0.0447 Y-0.1167
G1 X0.0447 Y-0.1167 Z0.1000 F40.
G3 X0.0000 Y0.0000 I-0.1115 J0.0509
G0 Z0.1250
G0 X0.0000 Y0.0000
M5
G53 Z
X0Y0

I ran the above code thru my wincnc simulator with the same result. Arc error on the G3 line.
I believe G3 is only to make an arc of 360 degrees or less. It starts @ the current X Y position and makes an arc around the center which is "I" distance away along the "X" axis & "J" distance away along the "Y" axis and stops @ XY if given or makes a full circle. If XY are given they must fall along the arc.

The I & J values give you a radius of .1226 & put the center of the arc @ x = -.0703 , y = -.0658.

Your toolpath intersects x=0 @ y=-.16625 & y=.0346
The toolpath never intersects x=0 y=0 therefore you have an arc error.

The following will cut a .75 dia pocket with its center @ X0Y0 using a .25 cutter

G0 x.25y0
g1 z whateverf40
g3 i-.25j0 f40
g1 x.115
g3 i-.115j0 f40

Of course I took an ambian 2.5 hours ago, so medicaly I'm asleep & this is a dream[lol]

[Eric Mims]

I wanted to post an update as I figured out what the problem was yesterday.. after all this time.

Wincnc has a particular way it wants arcs to be programmed. Yesterday I was cutting some letter profiles and in Rhinocam I have it checked to output arcs as arcs (as opposed to a bunch of tiny straight line segments). Well you end up with something similar to my first post, with the G2 or G3 command and XY and IJ settings. That's all fine, except my post processors in Rhinocam that were sent to me to work with Wincnc, had the settings for circles/arcs wrong.

It was outputting the start XY, and I and J were absolute coordinates, absolute to the table. It would give an 'error arc radius' in Wincnc everytime on any circle, arc, or helix. I changed it where the IJ was a coordinate that was relative to the start point of the arc, output as a vector from the start to the centerpoint of the arc. Also, I set the post processor so it was not modal on G2 G3 commands.

Voila, seems to work now.. I can tell you without hesitation that if you are not cutting using arcs, you will want to try it. I believe Wincnc has special accel/decel curves for traveling through a true arc. I tested it on the letter O, aircutting to see vibration in the machine because I had been getting chatter marks. Even using a really high G9 smoothing number like S85, it still stuttered slightly. I reprogrammed using arcs (and mind you, it was not just 1 or 2 arcs to make up the odd shaped 'O', it was maybe 20 with a few tiny straight lines in there too. The file cut so smooth, really nice!

[pescado_loco]

That's the trouble with post processors. It's really hard to figure out what they are doing wrong. Especially with complex code. I allways write straight forward code manually to try to keep it straight in my head how each code works. Then when the complicated stuff from the post processor does not work, I have a small chance of figuring out what is wrong.

Merry Christmas!

[Eric Mims]

Well the interesting thing is that I never could find anywhere in Wincnc literature where it gave an example of what it wants/expects in regards to arc code. All it would take is a simple picture with a sample line of code.

[pescado_loco]

For the price on Wincnc, one would think it should be alot better than it is. The things it does it does well, but a few more G & M codes and some documentation would be really nice.

[Eric Mims]

yea, actually, with the latest release of their manual from their website, it isn't too bad. Just some things like this are just not very clear.

[james mcgrew]

i know this will sound wierd and we can fault them or we can help them. the original owner sold this company (wincnc) to the current owners, most all of the end users were institutional commercial manufacturer's who do not utilize this software controller the way most of us in the mid weight cnc machine owners do. in other words most of them were making the same thing over and over and over. then came the camasters, cnt and shopsabres machines and this started reaching the more talented (eric for example) as far as the manual it has never been misrepresented that it was written for a tech geek in a plant and not for us, they have done some improvement but only with our help after the last round (the great gecko fiasco) they "the two kelly's" have always been responsive to what we have asked, but unfortunatly the biggest portion of thier customer base is not us.

i will say this it is a stable controller and i have not had an iota of problems with it. the blue company and most propietary controllers are many times having rewrites due to bugs and other problems, this has not happened with wincnc.

lets let them know what we need and joey can get it to them or just email direct to wincnc and let them know. eric i always benefit when you find this stuff we all do thanks

jim

[mezalick]

Jim,
As one who is waiting for my new machine ( soon I hope) what can you suggest I read up on so that I can hit the track running?
My old machine ( Shark Pro) was pretty straight forward. The new Camaster is a big step up. I want to be ready for everything.
Any suggestions?
Michael

[pescado_loco]

I've emailed them several times asking if they had plans to add specific g codes like g17 - g19 that I really need. I have yet to get a responce from them. For the price of their package they should support & be responsive to all their users. If they aren't going to upgrade their software to add functionality, then they should at least have the courtesy to say so.

[james mcgrew]

wincnc responds to the oems, pescado contact your machine company for this. i have been under the impression you purchased a used machine of another brand. wincnc is very responsive to this contact joey for this response.

jim

[jkindelspire]

I wanted to post an update as I figured out what the problem was yesterday.. after all this time.

Wincnc has a particular way it wants arcs to be programmed. Yesterday I was cutting some letter profiles and in Rhinocam I have it checked to output arcs as arcs (as opposed to a bunch of tiny straight line segments). Well you end up with something similar to my first post, with the G2 or G3 command and XY and IJ settings. That's all fine, except my post processors in Rhinocam that were sent to me to work with Wincnc, had the settings for circles/arcs wrong.

It was outputting the start XY, and I and J were absolute coordinates, absolute to the table. It would give an 'error arc radius' in Wincnc everytime on any circle, arc, or helix. I changed it where the IJ was a coordinate that was relative to the start point of the arc, output as a vector from the start to the centerpoint of the arc. Also, I set the post processor so it was not modal on G2 G3 commands.

Voila, seems to work now.. I can tell you without hesitation that if you are not cutting using arcs, you will want to try it. I believe Wincnc has special accel/decel curves for traveling through a true arc. I tested it on the letter O, aircutting to see vibration in the machine because I had been getting chatter marks. Even using a really high G9 smoothing number like S85, it still stuttered slightly. I reprogrammed using arcs (and mind you, it was not just 1 or 2 arcs to make up the odd shaped 'O', it was maybe 20 with a few tiny straight lines in there too. The file cut so smooth, really nice!


I've been trying to get G2 and G3 codes to work following your steps here. I'm also using RhinoCam, but I cannot get WinCNC to run any G2/G3 commands without editing out the X and Y coordinates within the line. Even then, I don't get the results I want.

Eric- Can you post your PP settings for RhinoCam?

TIA,
Justin

[Eric Mims]

simple gcode from an engraving operation of a 2" square with .25" radius corners; corner at 0,0. The PP I use for my X3 is zipped up, out in your rhino/plugins/rhinocam/post directory and check it out. some settings might need to be tweaked for your machine, but this works great for mine.

G90
T1
S10000
G0 Z0.1215
X0.0000 Y0.2500
G1 Z-0.2500 F100
G3 X0.2500 Y0.0000 I0.2500 J0.0000 F100
G1 X1.7500
G3 X2.0000 Y0.2500 I0.0000 J0.2500
G1 Y1.7500
G3 X1.7500 Y2.0000 I-0.2500 J0.0000
G1 X0.2500
G3 X0.0000 Y1.7500 I0.0000 J-0.2500
G1 Y0.2500
G0 Z0.1215
M5
G53 Z
X0Y0

[jkindelspire]

Thanks Eric.

I used your post processor and it appears as if G2/G3 will work. I'm not exactly sure what the differences were between our post processors, but it must have been minor.

[Eric Mims]

it took alot of trial and reading for me to come up with the a post processor that works just right for my machine. I'm quite sure more could be done to it.