plunging ramp or helix

[BOATDUDEGUY]

Something I may get into shortly and wanted to get the expert opinion s of the emastercam community

 

Wat kind of surface footage is agood starting point for ramping into carbon steels

Also witch is the better tooling for something like this solid carbide or indexables

Or is a helix entry preferred, either or? Also curious of wat deg of entry is best

[gcode]

what kind of machines are you running and what size tools are you planning to use?

[BOATDUDEGUY]

Mori vertical im not sure just yet im just spit ball n

1/2 for roughing poops n giggles

[cadman2112]

"carbon steels"

 

Well, that does open up a world of different possibilities.

 

So I'll be very general

 

I will typically helix entry 75-80% of my feed rate generally at a 2 degree. Now you're tool choice and exact metal being cut will determine much more of the exact cutting conditions.

 

On those occasions where I just cannot fit a helix in, I will ramp, again at a 2 degree zig and zag.

[BOATDUDEGUY]

Ya im just lookin for general s to start with, but do you only bring down the feed, and keep the speed same?

[cadman2112]

Typcially I keep the speed the same as that is tied to the SFM to you machine the material.

 

 

But lowering the feed rate decreases the chip load

[EX-wccprogrammer]

Are you looking for performance? Or are you going to use standard tools? Helical entries are more efficient than linear ramping. The bottom geometry on the tool dictates the allowable entry angle. I prefer solid carbide over indexable and try to use high performance where feasible.

 

One of my favorites in mild steels: 5 Deg. helix 80% Speed and 60% feed. For 1/2 dia = 5623 rpm 74.4 feed. No stepdown, cut full depth. For 1.25 depth, takes about 2 seconds to reach depth. Then bump speed and feed back up to 7029 and 124.

[MotorCityMinion]

Same thing here, huge shortage of data so I wing it at 50% feed. 1.5 deg. for all steels works safe so far for helix entry. Helix bore, .006 to .03 depending on hole size and tool being used. Lately we've been eliminating start/entry holes altogether and using a ramp throughout the entire pocket, 1 way, and ramping the exterior as well using a depth value, not an angle and tool life has been great. So far, Mr. Rush has posted the closest thing to an actual formula that I can find on the forum. It's a topic that does not seem to get enough coverage anywhere.

 

Indexable Feed mill ramp and helix: Page 13, 14.

HTTP://www.mitsubishicarbide.com/mmus/catalog/pdf/b/b028a.pdf

 

I'm still looking for good data to use with solid carbide e-mills. Anybody care to post some links?

[EX-wccprogrammer]

Links:

 

http://swiftcarb.com/index.php/videos

 

http://www.swiftcarb.com/

 

Chart I use is attached.

 

RampMilll Speeds Ramp Angle.pdf

[MotorCityMinion]

For that Swift pdf... less flutes, greater chip clearance = steeper angle, makes sense. Quite a variation of values for the different materials being cut. Those appear to be some aggressive angles. I'm going to check these cutters out. Whats your take on them?

 

We typically use generic 4 flute cheap carbide, ALTIN, with most steels so my thoughts are the numbers in the PDF should be a safe starting point

 

Thanks for the links. That PDF goes into the vault.

[MotorCityMinion]

Hmmm, this video is private in IE and Opera. Even the youtube link blocks me. Looks like I need to create an account.

 

Ok, I went to Youtube directly and it works fine without a log in.

[EX-wccprogrammer]

If you have memory and rigid tooling (mill chucks or thermal) these are very high performance tools. They need to be programmed using Dynamic toolpaths, and if you follow the guidelines for engagement angle, they do well in everything that I have tried. (Aluminum and mild steel.)

 

The videos don't lie.

 

I also use regular carbide endmills when I am cutting castings or other unpredictable materials. Then I have to be back in the 2 Deg angle range, with multiple depths.

[EX-wccprogrammer]

Wow, they are locked. I have no idea why they would do that. I have my own copies of all of their videos, but hesitate to upload them.

 

I do like the tools, though.

[EX-wccprogrammer]

Go to YouTube and search rampmill. You will get some vids.

[MotorCityMinion]

The videos are impressive. We have a Makino S56 with the Haimer system but use it primarily for finishing hardened tool steels. We spend quite a bit of money on expensive ball nose cutters and do very little roughing on this machine. But I am going to put a bug in the ear of somebody that runs a rather large shop in the area and has the resources to experiment with this stuff. Chances are , he may already be aware of them.

 

PS: Swift-Carb has a channel on youtube, open to the public with over 20 vids. You just half to go to youtube directly and search for Swift-Carb

[BOATDUDEGUY]

Turns out it will be aluminum and thanks on all the input makes me feel much more confident in attempting this for the first time