Feed/speed for plunge or ramping

How do you calculate feed rate for plunging or ramping into stock?

I have had good success with slot and profile milling in XY at feed rates between .003 and .007 IPM. Where I have had some tool issues like snapped or clogged tools is alway the Z movements. Early on in my learning process, I became gun shy in the Z and generally baby things with feed rates of around 25% ramping or plunging movements.

Using these really slow Z movements works fine and I have not had any broken or clogged tools in a while but I want to learn and understand how theory behind programming Z axis movements.

As a rule of thumb, what do you use for your ramping or plunging feed rates?

Yeah I agree I am horrified of Z plunging and my tools always break on the plunge for slots. I have never heard of a good formula or practice on here but then again I haven't looked to much. It does seem different from XY programming.

Mark,
Two flute endmills are pretty good in a plunge, up to it's full diameter in depth. Deeper than that, I ramp the tool. 3+ flute endmills typically are not as good with a plunge, so in the case of using a 3+ flute tool, I always ramp, unless the depth is very shallow (i.e. for a finish pass on a pocket floor)

3 degrees is a good starting point for your ramp angle. Larger tools and two flute endmills can tolerate steeper angles.

As for feedrate, plunging with a two flute must be aggressive, otherwise you'll build up a lot of heat at the tip of the tool. (and wrap chips around the tool) I typically start with 1/2 of my normal feedrate for plunging with a two flute endmill. If I choose to ramp down, I always use full feedrate.

Justin

Thanks!

Justin,

Once again BIG thanks!

Last week my Z plunge was 2ipm. This week I used the same tool to plunge at 20ipm while (using 600sfm and .003 fpt). It really feels good to see the machine perform better and bring my cycle times down. (actually it is not a ramp but rather a step down for my roughing cycle so the tool is not fully surrounded by material). In any case, I am cutting faster and feel good about the quality.

My pocket entry is now ramping at 3 degree with .004 fpt.

-Mark

Glad to help Mark.

To give you an idea of the limits, we were running parts last week, plunging at 150 ipm, then feeding at 320 ipm...but it was a really shallow pocket only going 0.15" deep. (12,000 rpm, 0.5" diameter endmill, 2 flutes) If I had more rpm, I'd go even faster.

Hope your parts are selling well. Don't hesitate to call/write, or swing by the shop if you need any help with troubleshooting...I know your parts are very challenging.

Justin

Quote:

---

Originally Posted by mrk

How do you calculate feed rate for plunging or ramping into stock?

I have had good success with slot and profile milling in XY at feed rates between .003 and .007 IPM. Where I have had some tool issues like snapped or clogged tools is alway the Z movements. Early on in my learning process, I became gun shy in the Z and generally baby things with feed rates of around 25% ramping or plunging movements.

Using these really slow Z movements works fine and I have not had any broken or clogged tools in a while but I want to learn and understand how theory behind programming Z axis movements.

As a rule of thumb, what do you use for your ramping or plunging feed rates?

---

This is a 2 part question. For ramping I use 100% speed and feed with a ramp angle of 3 degrees. When plunging, I use a 50% feed rate at 100% spindle speed int solid material with a centercutting tool. I can do this all day long in any material up to 40Rc.

When roughing with my high feed cutters I ramp in a circular motion at 2 degrees using my feed rate of 300" per min as my ramp speed. I NEVER plunge straight down, if there is not room for a circular ramp, then I will zig zag my way down at the same 2 degrees. My peck depths are between .025-.05 deep per pass.

I'd not ramp or plunge at all. (depends on CAD) Why don't you simply drill a pilot hole?

Ok I just realized the thread is nearly 10 years old :D