Overriding feed rate on first cut only

[OOZ662]

I'm doing a simple project that only involves making cubic pockets in X2 MR2 mill. I'd like to have the first cut of each pocket much slower than the rest, since the whole of the bit is engaged and it's overheating (no coolant here, and it's wood).

 

Any way I can do this with toolpath parameters or even editing of the posted file?

[edmBosto]

Wood? Cool! I would try a ramp entry 1st.

You can do a change at point also. Look at your lead-in tab in your TPath parameter page I believe there is a place to change some entry parameters. I never needed to do this, but take a look anyways.

[OOZ662]

I haven't a clue what the deal is. Mastercam's feed rate calculator thing says I should be able to run this three to four times faster than I am, but if I do the bit heats up, discolors, and eventually begins chirping. The heat seems to be damaging our spindle motor too.

 

(Side note; don't cut plywood with HSS. =P)

[edmBosto]

All I know is that if I was cutting square pockets in wood I'd use a 2 flute end mill so the heat build up is minimal with air to get the chips out. I would then use a smaller cutter to get a smaller corner radius if needed with a remachining toolpath. I would also ramp the cutter in. Unless I don't understand what your trying to accomplish.

quote:

---

since the whole of the bit

---

What are you using for a cutter now? Maybe the cutter should be smaller. With a 2 flute you can even do a plungecut at a slower feedrate right down to the bottom depth. Program it as a seperate tool path if you need to but it can be done in one as far as I can see. HTH

[cajahawa]

What type of wood are you cutting and how deep are the pockets? 2 Flute router bits work great if you don't have to cut too deep. Also, don't try to take too much depth at once. Usually I'll only take about .25- .3 depth of cut. You should be able to run 300-500 ipm. at that depth, depending on spindle speed. If your spindle is under 10000 rpm you will need to back off the feed.

[OOZ662]

I'm cutting press board with a 2 flute 1/4" HSS flat endmill bit, cubic pockets with a depth of .3 inches. I'm cutting at a feed rate of "30" or less (I don't even know what that translates to in "real" units). I really can't figure out what is wrong.

 

Can you go into detail of how to and what "ramping the bit in" means? I don't have Mastercam handy at the moment, so I can't see what you mean.

[edmBosto]

Ok try this in your pocket toolpath.

 

In the roughing/Fininshing Para. tab set:

z clearance : .1

XY clearance: .1 (If you have the room between tool and geomtery)

Plunge Zig angle: 3

Plunge Zag Angle: 3

If ramp fails : Plunge

Entry feed rate: Feed rate

 

Give this a try and watch it back plot 1st. With these settings it will only ramp if there is enough tool clearance.

HTH

[cadcam]

I cut this with 2 flute carbide about 7000 rpm and 100in min. But I also use Air on the tool.

 

As for ramping . if you are using the pocket tool path. on the last paramater page on the upper right side you will see the option either for Ramp or it might be set for Helix, use this button to set for Helix or Ramp.use ramp with a added width to give room for chips and not full ingagment with the tool.

[Goldorak]

try high-speed pocketing and set the trochoidal cut to off

 

this will put a ramp-in in each pass

[OOZ662]

Setting it up to ramp makes a very odd result; the bit wants to cut the first two pockets the same as before, then wants to "wiggle" down into the middle of the third pocket, then continue cutting just like before.

[Todd Tracey from Fastech]

This is on a Techno (Small) CNC Router I'm guessing. Where do you have the spindle speed set at? Slow it down a ways on the RPM. Probably below mid range on the dial on the spindle motor.

Is this a 8" X 10" or a 10" X 12"? machine

[Matthew Hajicek - Singularity]

Carbide cutters with edge prep for aluminum seem to work pretty well on wood. The "wiggle" is what you want, that's the ramp entry. Try turning down the x-y clearance to get it to ramp in the other two pockets. Personally I like the helical entry better than the ramp, 'cause you're not rubbing the sides then. I set min rad. to 25% and max rad. to 50%, so there's no boss left in the middle.

 

If you just want to change the feedrate on that first move, you need to right-click on the operation and select the last option in the menu that pops up: "Toolpath Editor".

[OOZ662]

The "tray" will hold 10x12, but will only cut about 7.5x9x3 with a very short bit.

 

The "wiggle" is only about a centimeter in length...and it starts what looks like an inch over the top of the piece and slowly winds down.

 

I'm so new at this it's not even funny...I'm trying to get enough interest in this machine that we can add an entire CNC section to our CAD classes. Obviously I have a way to go. Thanks for the help so far.

 

I'll mess with it some more tomorrow.

[Tom Dorgan from American Precision]

It is starting above the part because your Z clearance is set to 1.0 in the pocket parameters. At 30 IPM you are rubbing the tool and burning. You have to cut that stuff or you can start a fire. I ramp and cut at 300IPM with a .25 bit in press board @ 24000RPM. If I am plunging or doing a helix entry usually about 150IPM on plunge and then 300IPM feed. I also normally use a 30 deg ramp angle on wood & press board. A 3 deg angle takes forever.

[OOZ662]

Everything results in the bit ramping a hole about 1cm in width, then resuming the normal pocket cut. I need to ramp the whole first "line," don't I? the bit overheats while engaged with more than the usual cutting amount.

[OOZ662]

I've discovered that I've been running the spindle at the "medium" speed and only cutting at 35 IPM and 16000 rpm, but you say I ought to be able to do over 100 IPM. The best I can do clearing-wise is a shop-vac on the bit. We don't have the cover and blowing this dust all over isn't an option where I'm located.

 

EDIT: I just reread the above post; will cutting faster really do the trick even though I'm sucking the dust/bits immediately out of the way? I can't afford new bits and if part of this machine bites it, I'm done for.

 

EDIT2: Max speed for a one-axis linear cut on this machine is stated as 140 ipm. The spindle speed varies between 8 and 24 thousand RPM.

 

[ 02-01-2008, 04:41 PM: Message edited by: OOZ662 ]

[3R!< W3NG3R]

would the high speed toolpath with tricoidial cuts help here? this would get rid of the full cuts.

[OOZ662]

High-speed with tricoidal cuts looks like it could be helpful. I'd like to make the circles a bit bigger...but I've run out of time today. Any help with this or feed rate/spindle speed would be appreciated.

[Todd Tracey from Fastech]

You have 2 methods of controlling cut speed with the Techno. One is to use the "Programmed" feeds put out by Mastercam, the other is to use the Techno software to set the feed rate and use the function keys to speed up or slow down feed on the fly. It is set in the techno software setup to override or not. This is a Stepper system and cannot move all axis at the same time. It moves or steps each axis independently one at a time. They state 140 inches feed max, but that is one axis in a straight line. As soon as you try moving 2 axis or 3, it slows way down 35 IPM max would not surprise me. This is a limitation of the machine and part of the way they keep the cost down for schools. I sold Techno in education for several years, so I am quite familiar with their operation. The 10 X 12 table can be removed if additional Z travel is needed for a project. Just make sure you check alignment when you re-install it.

JM2C

[OOZ662]

Still, would the tricoidal cut give the bit what it needs to complete the job? Should I really crank the thing on spindle and feed rate?

[Todd Tracey from Fastech]

You are never going to acheive the feed rates some of the guys are reccomending with the stepper. You might find a 2 flute carbide would get you what you want. Other than that it may take some experimenting on your part. The limitations on doing arcs would really slow things down on the stepper so trochoidal would really not work well IMHO.

[OOZ662]

Speed isn't really an issue, as I have a year and a half to pump out 30 pieces. I just need to know how to do it without setting fires...again.