G64 Code Smoothing Explain

[artracing]

Can someone explain what G64 smoothing actually does.

What parameter controls the corner entry speeds of speeds going into a radius.

Rob

Similar Threads:

• Explain to me G- code please. I have an example from solidworks.
• Need Help!- smoothing surface
• Need Help!- G-code speed smoothing
• Smoothing 3d arcs?
• crash during smoothing

[cnckeith]

basically G64 rounds the g code geometry and the G64 parameters adjust how much rounding to do. i use it on my short vector high speed cad cam generated g code programs so i can run faster and smoother. it takes some trial and error to get the settings to get the results you want as not all g code programs and machines are the same.

[artracing]

basically G64 rounds the g code geometry and the G64 parameters adjust how much rounding to do. i use it on my short vector high speed cad cam generated g code programs so i can run faster and smoother. it takes some trial and error to get the settings to get the results you want as not all g code programs and machines are the same.

Thanks again. I have Centroid on a gantry router. This looks like it will calm down the jerkiness I have running 250ipm,

Once you set parameters you simply execute g64 to turn on? Only turn on where you need it, or global.
I have to get manual out when I get to my shop.
Any parameter advice?

Rob

[cnckeith]

you can turn smoothing on globally or use G64 to turn it on and off just in the part of the g code program you want. I don't use it globally, i insert the G64 in the g code with the editor where i want it to turn on. see the operators manual for into on how to use g64 in a g code program. http://www.centroidcnc.com/downloads...tor_manual.pdf

there is no one size fits all parameters..but i can suggest a starting point if you post a report.zip file from the system so i can see turns ratios and other machine specific parameters. also is this machine have AC servos or DC servos?

[artracing]

I'll insert where I need it. I'll post report later. Thank you.
I have D.C. Motor. Controller m15

[cnckeith]

here is starting point.
Ad2 in

221 20 to 1 (adjust as needed, depends on g code)
222 .01” to .001” (adjust as needed..depends on g code)
223 400
226 10 to 2 (adjust as needed, depends on g code)
227 95 to 60 (angle adjustment)
228 0
229 0
230 1
231 1

[artracing]

Perfect
Thank you
I'll try it today

Rob

[artracing]

Perfect
Thank you
I'll try it today

Rob

[mactec54]

Can someone explain what G64 smoothing actually does.

What parameter controls the corner entry speeds of speeds going into a radius.

Rob

Depending on your control as to how this is intended to work, G64 used in a Fanuc control and most others is to cancel a G61

For Fanuc and Fanuc-compatible controls, G61 is the modal exact stop check command. Note that G61 is cancelled by G64, which places the machine back in the normal cutting mode. There is also a non-modal exact stop check command (G09).

[cnckeith]

the centroid g64 has some nice features on how you call it and how to turn it on and off in the g code program. check this out.

[mactec54]

the centroid g64 has some nice features on how you call it and how to turn it on and off in the g code program. check this out.

That is the normal way to use smoothing in any control using a P0 call is a standard through out the industry, this is not special to just Centroid it is the standard that most manufactures use, the P0 is not used so much now in modern machines with a million or more Encoder counts per rev, these machines are already very smooth, the jerk factor is mostly caused by the lack of encoder counts, and the quality of the servo motors being used

[cnckeith]

yeah.. what i was referring to is....the way centroid facilitated the ability to call presets..so you can call a predefined smoothing preset or a custom preset, i use this all the time as I have different smoothing parameter setups for different types of jobs..sometimes even in the same g code program.
also since you mentioned encoder counts.. at this day and age we still use the G64 feature even with the latest servo and encoder technology like yaskawa sigma7 equipped machine tools..the reason... it allows user to 'fix' dirty g code output from some cad/cam system. often in short verctor 3d and 5axis cad cam g code output there are anomaly vectors that cause jerkyness since the control is doing exactly what the g code program has told it to do...G64 allows (to a limit) to smooth out 'dirty' short vector g code by preprocessing it and lofting arcs thru the short jerky vectors for best fit and best smoothness..