Slow down in corners

[George Gerhard]

Hello everyone

I am trying to help my customer with an old woodworking machine, that does not have the high speed machining options. I cannot remember but was there not a machine dynamic table to configure to get a slow down in the corners

version X4

 

thank you

George

[Toonz]

What brand is the machine? What version of control software?

[Nils N]

George, see this thread

[Nils N]

Oops this thread optimize feed rates

[j.nguyen]

Nils N-

 

I live on the foss waterway at the end of the condemned bridge across from you. Let me know if you ever get into a jam and need some extra programming or designing help.

 

Jamey

[Nils N]

Just saw this Jamey, maybe we should have a beer sometime

[neurosis]

It would be nice if there was a slow down in corner option in the individual operations rather than having to use a global or the optimize feed rates.

[Superman]

Is there a G-code the would make the machine slow down or check its position like an "Exact Stop" function ?

 

If found, it could be incorporated into Mastercam using Misc Intergers, so you could leave it OFF for roughing, but have it ON for accurate work

[kunfuzed]

Slightly off topic, but I wish there was a way to slow the tool down in arc moves depending on the size of the tool and radius being cut. Refering to this formula.

 

ArcF = LinearF (HoleR - ToolR)/HoleR

[Leigh @ Kodiak]

quote:

---

Slightly off topic, but I wish there was a way to slow the tool down in arc moves depending on the size of the tool and radius being cut. Refering to this formula.

 

ArcF = LinearF (HoleR - ToolR)/HoleR

---

I'm betting this could be done by customizing your post

[Superman]

I know that Okuma has this ability in their parameter settings since the 90's.

I'm confident saying that most modern CNCs would have this ability too.

 

All you have to do is find it

[35K chipper]

Superman,

this is how i control my okuma's U100M control.

 

phinca # Super Hi-NC Control Selector

if mi8$ = 1, "G131J0I0", e$

if mi8$ = 2, "G131J1I0", e$

if mi8$ = 3, "G131J2I0", e$

if mi8$ = 4, "G131J0I1", e$

if mi8$ = 5, "G131J1I1", e$

if mi8$ = 6, "G131J2I1", e$

if mi8$ = 7, "G131J0I2", e$

if mi8$ = 8, "G131J1I2", e$

if mi8$ = 9, "G131J2I2", e$

if mi8$ = 10, "G131J0I3", e$

if mi8$ = 11, "G131J1I3", e$

if mi8$ = 12, "G131J2I3", e$

if mi8$ = 13, "G131J0I0K1", e$

if mi8$ = 14, "G131J1I0K1", e$

if mi8$ = 15, "G131J2I0K1", e$

if mi8$ = 16, "G131J0I1K1", e$

if mi8$ = 17, "G131J1I1K1", e$

if mi8$ = 18, "G131J2I1K1", e$

if mi8$ = 19, "G131J0I2K1", e$

if mi8$ = 20, "G131J1I2K1", e$

if mi8$ = 21, "G131J2I2K1", e$

if mi8$ = 22, "G131J0I3K1", e$

if mi8$ = 23, "G131J1I3K1", e$

if mi8$ = 24, "G131J2I3K1", e$

 

i have all the options predefined in the control

then i select the fidelity in need in the operation. at the end of the op it cancels with a G130.

 

35k [big Grin]

[Superman]

Yeh, I know about the tolerance control, and Supernurbs, but on the older machines, they don't have it, and a good workaround was to have G64 ( I think ) manually inserted in a finishing operation to stop the machine rounding or choppig out the internal fillets, beats puting in a slow feedrate for the entire pass or running it thru Highfeed optimise, as the G-code could be inserted by the operator ( if it was needed ).

[Alvaro Gil - Cimquest-inc.com]

under pcirc you can throw in a line that says:

 

if mr10$, feed = feed*mr10$

 

then you can throw in a multiplication factor in the misc reals to cut down your speed by. This would solve the problem for contours or pockets.

 

I have a customer that needs this simple functionality. HighFeed/HighSpeed is too complicated for him and it lengthens the code to much for his non-drip feeding controller. So I understand peoples pain with the current methods.