Speeding Up CNC Feed Rates Around Corners
Advice on how to safely tweak the cutterhead feed speed up when routing corners, to prevent burning. September 27, 2008
Question
We are running a Jet3006 with Genesis 2.2.5 and autolink software. How do you adjust the feed rate of a route going around outside corners? The default value is very slow and slightly burns the corner.
Forum Responses
(CNC Forum)
From contributor M:
You are probably making an arc move at the corners, or rolling around them. This would be a circular call G02/G03 at the corners regardless of the angle. For many machines, this is not a problem and is not even noticed by the casual observer. Since the radius would be small, you are getting a slower feed through the corner. If you can get the software to make straight moves on non-acute angles, then your feed will be much faster. I hope this helps.
From contributor M:
If you're making square cut around the corner or very small radius the feed is controlled by the servo drives parameters. There are acceleration and deceleration parameters that drive axis depending on the programmed feed and parameters inside the drive. Basically, PLC is calculating the direction and angle at which is going to change on the next move and makes adjustments.
I would suggest if you are making linear (square) cuts go past the corner if possible (Lead-Out), return back and make Lead-In an inch or so before the entry point. If you're making radius cuts make sure your radius is tangent to both lines connected on each side of the radius and make it as big as allowed by the design.
From contributor B:
In the Control Editor, where the set mill information is found for your program, there is an Fr entry area. The value that goes in the Fr area is the minimum speed for direction change for outside cuts, for the most part, to keep from burning the corners.
Each set mill will need to be modified that is followed by an outside corner, or you can change the layer convention used with AutoLink to enter this information for you.
Unless you put a value here, the control defaults to a setting that will give the super slow corners, along with far more accuracy than is generally needed for woodworking. If you are programming in millimeters, something around 2.5 would be good. If you are in inches, 100 or so will work.
From the original questioner:
In the control editor, the Fr box is checked "auto". Is there a way to change what this auto default value is, or do I have to override it every time?
From contributor G:
Look at your code at the corners and increase your "F" to a larger number.
From contributor K:
Open the Technological Parameters program, click on the button in the tool bar that looks like a stop-watch (working feed), and increase the field for "Inserted Fillet Feed". This will be the global change that you are looking for. You may need to initialize for this change to take effect.
From contributor M:
I would be very careful about changing feed rates in the parameters (not programmed feeds) to the level where it is not known how is the machine going to be affected by it. There are physical limitations of the machine axis and the inertia of the machine frame makes it worse when machine rapidly changes the movement direction. Most machines have something called Axis error or Threshold or something like that where machine checks the programmed vs. observed (actual) position value. If it is beyond the threshold parameter it will give you an error and/or E stop.
From contributor I:
Contributor K is absolutely right about setting the global parameter. You will want to set it somewhere around 100" per minute for your corners. Check the quality on the first couple pieces and adjust up or down to your needs.
From contributor A:
As Contributor B said I would make the adjustments in the Program Editor in the Fr box. I tried the Global Parameters once before and found that it would make the larger diameter tools move around the corners way too fast. 2 - 3 meters per minute in the Fr box works really well for me. That setting seems to work well from CNC90 to Evolution.
