Rules for slowing down in corners

[2strokeforever]

I am trying to figure out how to slow down in a more linear way for tight corners or holes.
Let's say I am slowing to 60 percent for holes smaller than 1 inch.
That might be too slow for 1 inch and too fast for 1/4inch.

Is there a way to make it proportional?
Can I do a series of rules where
60% smaller than 1"
50% smaller than 3/4
40% smaller than 1/2
Ect
Will this work, will the slowdown percentages add up for each rule or will it pick the best fit?

Just want to see how everyone else is dealing with this

[acourtjester]

One thing to look at is the fact that the more you slow down the more dross you create. I do not think you should look at a proportional speed change by hole size. With testing find what speed works and use that for all sizes. IMHO Also the slower you go the more heat you put into the metal, thin metal may warp to much.

[2strokeforever]

I know on thick plate there is no speed that works for all sizes.
I guess you're right on thin plate most of that slowdown isn't needed.
I can't have it slowdown to 30 percent at .99" and be 100 at 1 inch, that's not consistent and won't produce a nice finish either.

My issue is most noticeable cutting 1" with my powermax 65. Dosent seen to matter much with 3/16.

[adbuch]

I would consider simply creating the cut paths for the holes and the cut paths for the remainder of the part separately (I would call them layers, but I know there is a proper SheetCam term). Then you can tailor the cut speed for the holes to your liking.

I happen to have a Plasmacam table with Design Edge software, and there are settings for corner acceleration as well as "slow on holes/curves under a certain diameter". The reduced speed is proportional to the square root of the diameter of the circle. So this is sort of what you would like to do with SheetCam. You might ask Les over on the SheetCam forum for more information about this.

David


This is from the Design Edge manual describing how the corner acceleration and "slow on circles under" works.

[djreiswig]

There are path rule options for corners, arcs & circles in SheetCam. You can adjust speed by a percentage and also turn the THC on or off a set distance before or after the location. You can also run different codes in the path rule.

[sheetcamCS2]

I agree with all the advice given.
Here is a test case that demonstrates reducing feedrate on 3 different circle diameter limits using 3 rules.
I used a base feedrate of 1000mm/m so its easy to see the percent of reduction in the gcode, and arbitrary reduction percentages in the 3 rules.

btw- I should add that the diameter which triggers the rule is the toolpath dia, not the shape dia. Thus a for a 10mm dia rule, and inside toolpath will trigger it, an outside toolpath will not (not the 10mm rule, but the latter will trigger the 20mm rule).