EMC2 error message

[lancut]

Hi, I generated a gcode in CamBam plus version and EMC2 is complaining that the " Radius to end of arc differs from radius to startline". Can sameone point me where the problem is. The code runs great in NCPlot simulator. According to the people on the CamBam website there should be a way to set the "Arc Center Mode" either Absolute or Incremental. I have look anywhere in the config.ini file and Hal.ini (not sure I got those right)and can't find anything pertainig to an arc mode... Any suggestion, newbee willing to try anything.

[acondit]

The usual problem for that error is that emc2 is set to tighter tolerance than NCPlot, hence NCPlot accepts the code but emc2 rejects it. My recollection is that there is a gcode that will change the tolerance in emc2, but the better approach is to determine what the radius offset should be and fix the code that way.

I often found that if I really zoomed in on the start and end of arcs they weren't precisely where I wanted them, or I had the precision spec in my drawing set so that it was rounding to the nearest thousandth rather than the nearest ten thousandth.

Alan

[jmelson]

Originally Posted by bronek Hi, I generated a gcode in CamBam plus version and EMC2 is complaining that the " Radius to end of arc differs from radius to startline". Can sameone point me where the problem is. The code runs great in NCPlot simulator. According to the people on the CamBam website there should be a way to set the "Arc Center Mode" either Absolute or Incremental. I have look anywhere in the config.ini file and Hal.ini (not sure I got those right)and can't find anything pertainig to an arc mode... Any suggestion, newbee willing to try anything.

EMC uses the I,J words as incremental offsets to the center of the arc. There may be two ways to fix this. First, see if CamBam can put out more digits to the right of the decimal point. If your numbers are like X1.234 I0.456 see if you can bump it up to at least 4 or 5 digits.
Another way to fix this is to set CamBam to put out the arc radius as an R word, so instead of
G02 X1.234 J2.345
it writes it as
G02 X1.234 R0.456
By sending the arc radius in the R word, there is always an arc that will fit the parameters, so you can't get that message. What it is telling you is that when it measures the radius length from starting point (where the last move left the machine) to the arc center (specified by the I and J words) and then measured from that center to the end point specified by the X and Y words in the move, those radii differ by more than the tolerance that EMC allows.

You can also change the start/end radius tolerance for arcs, it is somewhere in the manuals. But, first, you should make sure CamBam is specifying the coords to sufficient precision for your needs before relaxing EMC's tolerances.

Jon

[lancut]

With all you fellas help I got it solved. Changed the setting for the "Arc Center Mode" in Cambam to absolute and that was it. Thanks.

[0die]

Hi guys, I had a similar problem.
I'm using Ace Converter to convert my TurboCad .dxf files to g-code .nc files.
The error was avoided by increasing the Precision settings value of Ace Converter.
I assume this means that my milled items are now a little less accurate. I estimate around 0.05 of a mm

[jmelson]

Originally Posted by 0die Hi guys, I had a similar problem. I'm using Ace Converter to convert my TurboCad .dxf files to g-code .nc files. The error was avoided by increasing the Precision settings value of Ace Converter. I assume this means that my milled items are now a little less accurate. I estimate around 0.05 of a mm

Ummm, no, not LESS accurate, MORE accurate. The cause of the error is that EMC2 is very picky about the arc radius matching at the beginning and end of the arc. Depending on roundoff, if too few decimal places are supplied in the I, J, K words, then the distance from the center to the start and the end of the arc can differ by one least significant digit. By making the CAM system specify more digits of precision, EMC is satisfied that the distances match to enough digits. Some other CNC controls just "fudge" it, and guess by averaging what radius you meant to specify. EMC requires the radii to match pretty exactly. Another way is to specify the R word and give the radius exactly. This can never suffer from a mismatch.

Jon

[0die]

Jon, you are absolutely right. My apologies. After posting the answer I thought about it for a while and it would make more sense that the values would be more accurate and therefore accepted by EMC2. I was going to edit my answer but forgot about it. Thanks for the correction.