Circle mill toolpaths

[monty]

Hi Guys,

Don't you think in CIRCLE toolpaths we should be putting the required feed at the cutting point and Mastercam should be calculating the feed at centre of cutter in nc output depending upon cutter and hole diameter as we are never cutting in a straight line.

[Guest]

nope, very happy the way they are currently handled thanks

[Hardmill]

NO!!

 

 

PEACE

[Troy Gossett Indepak Inc.]

It seems like circle paths are the ones that have a constant angle(or percentage) of contact. If Mastercam was to calculate speed changes it would be the toolpaths that the angle of contact is constantly changing on like pocket and contour etc.

[heavychevy2155]

Good point Troy.

[monty]

quote

---------------------------------------------

It seems like circle paths are the ones that have a constant angle(or percentage) of contact. If Mastercam was to calculate speed changes it would be the toolpaths that the angle of contact is constantly changing on like pocket and contour etc.

---------------------------------------------

Not only that but feed could be 50 times more then required if differene between cutter dia and hole dia is small and this is nothing to do with speed or angle of contact as they stay same once cutter has started cutting the diameter of hole.

[DavidB]

I think it's a good idea Monty for circle toolpaths.

 

Save having to use this formula for caculating the correct feed rate.

IN LINE FEED = ((hole dia - tool dia) ÷ hole dia) x calculated feedrate.

[3R!< W3NG3R]

maybe they could add a calculator for the feed rates including some of these formulas. (kind of like the drilling depth calculator.

[monty]

I absolutly agree with you eric.

[Glenn Bouman]

Have you tried the "Adjust Feedrate on arc Move" in the Machine Group Properties, Tool Settings"?

[3R!< W3NG3R]

quote:

---

Have you tried the "Adjust Feedrate on arc Move" in the Machine Group Properties, Tool Settings"?

---

the only problem with this is that it is global.

[Roger Peterson]

It is not global. It only effects toolpaths created while it is checked. But, I'm not sure how slowing down the feedrate on outside corners of contours helps anyway. For circlemill it works, just make sure you have it checked if you regenerate at path that needs it (I lock these toolpaths personally).

 

I would love to see a "maintain chip load at edge of cutter" checkbox.

 

Edit:

 

something that was integrated with the machine def/highfeed filter that takes into consideration the cornering capabilities of each machine. Maybe part of the highfeed filter. Currently you need to calculate what you want the max feedrate to be, then the highfeed filter will slow it down when neccesary based on direction change (in finish mode). It would be nice if I could set the desired feedrate, and then it would increase/decrease based on my cornering capabilities as well as trying to maintain the chipload at the edge of cutter for both inside and outside corners.

 

 

JM2C

 

[ 01-11-2007, 05:42 PM: Message edited by: Roger Peterson ]

[monty]

Yes I tried Glenn, But insted of increasing the feed it reduced from 500mm/min to 128.1mm/min.

I am using a contour toolpath and I am milling a o-ring groove on a 20dia boss using 63mm convex slitting saw.

And another thing don't you think it should give us option for hole and boss.