faster feed rate = more gcode lines??

[a3dcreator]

Is it just me or is this definitely the case?
I recently noticed that my the contour i asked my cnc to do would not look like the contour I asked it to do.
The corners did not look like corners. They were like smoothed and rounded out. almost like if there was no corner.
Unless i lowered the feedrate to 40 IPM. So I decided to investigate.
Turns out that if I provide more Gcode lines or (more resolution) I could run it properly at that faster feedrate which was 200 ipm. else i had to run it at 40 IPM.

If this is true why is this the case? id like to understand it a bit more.

thanks!

Similar Threads:

• Australia feed rate and plunge rate help required please
• material removal rate: what's faster for the same thing? Mill or lathe?
• Need Help!- Feed rate Ovverride also Increases rapid rate.
• Feed Rate is not included in G01 lines

[ali_mak46]

Is it just me or is this definitely the case?
I recently noticed that my the contour i asked my cnc to do would not look like the contour I asked it to do.
The corners did not look like corners. They were like smoothed and rounded out. almost like if there was no corner.
Unless i lowered the feedrate to 40 IPM. So I decided to investigate.
Turns out that if I provide more Gcode lines or (more resolution) I could run it properly at that faster feedrate which was 200 ipm. else i had to run it at 40 IPM.

If this is true why is this the case? id like to understand it a bit more.

thanks!

What's your controller and what's the application you are using ?
If you are able to have a g code with more points do it. But this is only one of the possibilities or reasons
You can see your g code in some application like cimco before starting it
And while preparing g code toolpath make the points closer to each other and use less separation point distance


Sent from my iPhone using Tapatalk

[a3dcreator]

thanks for the reply. I was investigating some more and it seems like that might not be what fixed it. I think it might be something called undershooting or overshooting.
One other thing i changed was for every line I was setting a feedrate. in this new gcode i also only set the feedrate once. At the very beginning of the file. Im starting to believe that this might have caused my controller to adjust to the neccessary feedrate before it gets to that corner.
I will check tonight.

im using Mach4 controller. With Hicon Integra motion controller.

i will update you tonight once I get back to my machine.

[ali_mak46]

thanks for the reply. I was investigating some more and it seems like that might not be what fixed it. I think it might be something called undershooting or overshooting.
One other thing i changed was for every line I was setting a feedrate. in this new gcode i also only set the feedrate once. At the very beginning of the file. Im starting to believe that this might have caused my controller to adjust to the neccessary feedrate before it gets to that corner.
I will check tonight.

im using Mach4 controller. With Hicon Integra motion controller.

i will update you tonight once I get back to my machine.

Thank you for you reply
But there might be other reasons too if you can't have a smooth corner
Like inappropriate tool or spindle speed , hard material, or many different things
Or if there's not a suitable relationship between spindle speed and feedrate or even tool angle
Although it's still hard to fully imagine what's your part's shape.


Sent from my iPhone using Tapatalk

[ger21]

It's rounding corners for two reasons.
1) Your machine has a low acceleration rate.
2) Mach4 really has no method to control path deviation in CV mode.

[a3dcreator]

here is the image of the contour im trying to cut. its supposed to cut right on the center of the path.
The green is what i want to cut but it was doing the red path. Whats wierd is it would only do it on the first corner and not on the second corner. As illustrated.

[a3dcreator]

what is CV mode?
sorry for being so noobish.
and does this mean i should up my acceleration?

thanks!

[ali_mak46]

here is the image of the contour im trying to cut. its supposed to cut right on the center of the path.
The green is what i want to cut but it was doing the red path. Whats wierd is it would only do it on the first corner and not on the second corner. As illustrated.

May I see your G code ?
It seems that g code is not match with the machine
Or machine doesn't read arcs of g code properly
Or they don't have the same logic


Sent from my iPhone using Tapatalk

[ali_mak46]

what is CV mode?
sorry for being so noobish.
and does this mean i should up my acceleration?

thanks!

That's totally ok my friend
I don't know many things either
But about your problem i think the problem is around G2 and G3 if there is any in your g code


Sent from my iPhone using Tapatalk

[a3dcreator]

here are the 2 gcode files.
"contourTest2.txt" is the one that produces these artifacts.
"contourTest3.txt" is the one that actually works. (i added more gcode lines in this one. also does not have feedrate on every line.)

[a3dcreator]

by the way. im writing my own plugin that spits out the gcode from a peice of software called Autodesk Maya.
Ive managed to have access to a ton of information . I actually know when the path changes trajectories. so if i need to i can lower the velocity (or feedrate as it approaches the corner).
im just wondering if this is going to be necessary. And im also not using any arc moves in this gcode,

[ali_mak46]

here are the 2 gcode files.
"contourTest2.txt" is the one that produces these artifacts.
"contourTest3.txt" is the one that actually works. (i added more gcode lines in this one. also does not have feedrate on every line.)

Do you know all the parameters in your g code ?
Like G20
G94
And else ?
Are you expecting millimeters or inches in your size ?
I'm turning my pc on to check the g code more. Just give me time


Sent from my iPhone using Tapatalk

[ali_mak46]

by the way. im writing my own plugin that spits out the gcode from a peice of software called Autodesk Maya.
Ive managed to have access to a ton of information . I actually know when the path changes trajectories. so if i need to i can lower the velocity (or feedrate as it approaches the corner).
im just wondering if this is going to be necessary. And im also not using any arc moves in this gcode,

I guess that the problem isn't about feedrate now
It can be from the G code I suppose


Sent from my iPhone using Tapatalk

[a3dcreator]

other than G94 yes. my assumption would be that i should use G94 (units per minute mode)....
I am working in inches per minute.
thanks!

[ger21]

It's definitely due to feedrate, in conjunction with acceleration.

CV mode = Constant Velocity mode, where Mach4 tries to maintain velocity while following the path.
If you change to Exact Stop mode, you should see it follow the path exactly, but stop at each line of g-code.
Better control software allows you to specify a maximum path deviation while in CV mode.
When in CV mode, the faster the acceleration, the faster it can change direction, which allows it to follow the toolpath more accurately.

Mach4 does have a CV angles setting, where I think you specify a max feedrate for changes in direction based on angle, from 0-180°. Not sure how to set it up, though.

I would try to output your code using arcs wherever possible, as it will give smoother, and more accurate motion.

[a3dcreator]

thanks for the info. i wouldve never known

[samco]

This is what a normal machine control would look like with path following control

This 3 tolerances.
G64P.01
G64P.005
G64P.001

The above means - go as fast as you can but stay within P of the programmed path.
This control has a few other settings to - but this is the basic one.

This was at 200ipm with acceleration of 30in/s^2

Zoomed in


Zoomed out a bit.

[a3dcreator]

wow this really helps. So i have 2 solutions fortunatley.
I can either change the settings in mach4 and see if it works. or i can just change the feedrate as i approach the change in direction through my plugin and bake it into the gcode.
I will let you know how it turns out tonight.

[a3dcreator]

Question for you know is though.
if you had the ability to choose to fix the gcode and keep constant velocity or switch to exact stop. Which one would you choose?

thanks again!

[109jb]

Try just putting a G61 into the first line of the G-code. This is the exact stop mode and disables path blending, or should depending on the control software.