To Ramp or to Plunge?

[bborb]

I have a center cutting two flute diamond coated endmill that's a half inch in diameter and I want to circle mill 7/8 inch diameter holes in fiberglass without a pilot hole. A buddy said he'd plunge straight down about 0.1 inch and then circle mill the 7/8 dia., then plunge another 0.1 and then circle mill the 7/8, repeating till the whole was to depth.
This control (Fagor on MotionMaster iron) can interp 3-axis so I could helical mill to the bottom of the 1" deep hole, a constant "ramp" as I circle mill the hole.
Anybody have a recommendation which is a better approach to machine this hole? All comments welcome.

[keebler303]

I'm pretty sure that a helical path would be best. Plunging is generally avoided if possible. This topic has been discussed here several times maybe you could try the search function to find some older posts on the topic.

Matt

[Geof]

Probably fiberglass is soft enough it will not make too much difference but in metal I find the cutter tends to try and walk around when plunging fast.

My preference is to use helical interpolation.

I think the walking I mention is simply because the end clearance on the cutter is so small if you go down too fast it drags its heels.

[BobWarfield]

Out of curiousity, I tried ramping rather than plunging on my manual mill one day. It's a little harder because you have to walk and chew bubble gum at the same time, LOL. In other words, you have to turn 2 handwheels at the same time.

I mention this not because I was doing helical interpolation by hand on a manual mill! No, I was ramping in a straight line. I mention it because you could feel with your hands how much more nicely, smoothly, and easily it was cutting that a plunge. It was quite a shock to see what a difference it was making. If nothing else, it might flex your fiberglass less if that matters at all.

Now I always check the ramp box on my CAM program.

Cheers,

BW

[bborb]

Thanks to all !
Is there a "rule of thumb" as to the Z-feed versus the X-Y feed? Sort of the min/max of angle of ramping?

[PinMan]

Originally Posted by bborb Thanks to all ! Is there a "rule of thumb" as to the Z-feed versus the X-Y feed? Sort of the min/max of angle of ramping?

I use helical toolpaths all the time on my Fagor 8055, it really is great
As far as feeds, if you have a rigid enough setup, you can do 100% of the SFM. I cut that feed on 303 and 17-4 SS

[Geof]

Originally Posted by bborb Thanks to all ! Is there a "rule of thumb" as to the Z-feed versus the X-Y feed? Sort of the min/max of angle of ramping?

If you go too steep in metal you tend to jam chips into the flutes at the tip...and break the cutter. Then you back off.

Rule of thumb? In aluminum one third of the cutter diameter per circle(?); i.e. 0.500" two flute cutter doing a 1" hole make Z somewhere between 0.15 and 0.20 and halve this in steel using a four flute cutter.

This is the ball park I tend to stay in.

[keebler303]

I think if you plunge right in, you might delaminate the fiberglass on the back side a little more than if you ramp, if this is important.

Matt

[ALLtra Mach]

Helical interopolation is by far the best.
If you have manufacturers parameters they should list the maximum ramping angle of the tool. Other than that Geof's guidlines are pretty good.
With a laminate material you'll want to try and avoid seperating the laminations so too shallow can be as bad as too deep. You didn't mention whether the fiberglass was laminated or how deep. Like any other new tactic, start easy and work up to it. Practice on scrap.

[bborb]

Thanks again everybody. Seems ramping is preferred, and my search found most agree with a 3 degree ramp angle, some say you can go up to 5 degrees. I'll stay just below 3 degrees and start with a chipload of about .004 per flute unless somebody recommends an alternative ramp or feedrate. The spindle only goes to 1800rpm so I'll run it at that. I'm off to buy dust masks now since this router has no coolant, only air vacuum. Been thinking of those vortex cold-air guns to cool the tool.

[mactec54]

Hi bbob

Try this X0Y0 centre of hole cutter .500 hole dia .875 with a .06 arc off at the end this will give you a helix this is the coolest way to do any holes This is doing .1 per pass you can ajust what numbers you want


G43Z.1H1
G1Z0F16
G2X0Y.1875Z-.02I.1783J-.0579F20
Z-.12J-.1875
Z-.22J-.1875
Z-32J-.1875
Z-42J-.1875
Z-52J-.1875
Z-62J-.1875
Z-72J-.1875
Z-82J-.1875
Z-92J-.1875
Z-1.020J-.1875
J-.1875
X.06Y.1275J-.06
G0Z.1

[bborb]

Thanks mactec54, I hadn't thought of that .06 enter/exit strategy, good idea.