Hello, I have a small problem that I would like to solve, namely how to slowdown tool before entering an arc.
My tool path goes from a straight line into an arc and straight line out. Since im working with wood which is softer and where it matters if youre cutting paralel or perpendicular to growth rings.
I tried using "Adjust Feed Rate" which speeds the feedrate to double and "Feed Slowdown in Corners" which does not change the feedrate.
So I used the "Edit Toolpath" command, selected all arcs and set a slower feedrate(80) manually.
But this creates another problem, feedrate changes right on the entry into the arc which creates uneven arc and splinters since machine has to slow down from 420 to 80, while allready cutting the arc.
What I would like to do is that the machine would be stopping down before entering the arc and speeding back up after exiting the arc.
I added my file and a picture which is showing on which corners should the feedrate slow down and how the growthrings are positioned (black lines).
I did also try to divide the toolpath by plane but then i got 60 different toolpaths and the one toolpath i wanted to divide (straight line) was still intact.
Is there a way to do it like in the last picture? to cut a toolpath into 2 segments and then changing the feedrate?
Edit: I apologize, i didnt realize i didnt upload the whole part, i uploaded it now
Solved! Go to Solution.
The old feed slowdown in corners is looking for "corners". Since there are tangent arcs, it won't do a thing.
The system knows how to adjust feed for material removal, so I would try to use optimize feedrate. If you add some extra blanks at the corners, the system thinks the tool is coming in to more material, and will slow down the feed.
You forgot your component, so I made a part to demonstrate. I tried 2 options - a cylinder and a triangle, and added them to the blank. Then I told the system to optimize the feedrate. I set the nominal stepover and depth to the conditions along the walls, and let the system gradually slow down as it got to the corners. You can see the feedrates on the right.
I think if you experiment with the optimize parameters in the feeds and speeds dialog, and the sizes of the blanks, you can get what you want. Of course, if you do this a lot, I would look at some automated way to add the blanks.
if the part is prismatic, you can use Planar Mill operation and set different feedrate to each member of part boundary. So on arc you can set feedrate = 80.
See attached files, if it helps.
Hello, i did try adding blanks to corners, however it did not change the feed rate when generating toolpath with optimize feed rate enabled. Then I tried resizing the original blank box to smaller size since i thought its not slowing down becaouse the program thinks there is enough material infront of the tool as it is and adding cylinder blank doesnt change it, but after resizing the blank box it still didnt change the feed rate
you must play with Optimize Feed Rate parameters.
Attached is your operation with different settings parameters and it slowdowns feedrate from 300 to 170 in place where is cylinder.
You can divide the face where you want the different feed rate, so you can change it before the arc starts.
Attached you can find a picture.
Now I'm seriously confused, Ondra, when I load your edited part that you posted last it does indeed slowdown from 300 to 170. But then when I again open the same part but from my file, and edit the optimize feedrate parameters just like you did, it's not slowing down again :/