carbide rougher cutting info needed

[bll230]

I have not had good luck with 3/8 inch carbide roughers in my Tormach. The tips keep breaking off, even at very low feeds. The whole point of roughers is to remove metal faster, but if they keep breaking they are not very useful. I have tried RPMs of 1000, 2000 and higher, and feeds as low as 5 ipm, pretty much the tips break off all the time. Is the problem that 3/8 just doesn't provide enough material to keep the carbide from chipping?

I use ER collet holders exclusively, Hysol MB 50 coolant, and the steels I cut are soft, 12L14, 1018, etc.

Anyone have any suggestions on how to remove steel reasonably quickly?

 

[13engines]

It might help to include more information like flute length and stick-out. Depth and width of cut. Stuff like that.

My first guess is your machine or setup doesn't have adequate rigidity to run a 3/8 carbide rougher in any meaningful way. You could try CO/HSS and may have better luck.

As with any carbide, you have to create a real chip or take a cut of sufficient size to remove the heat from the work area/tool/etc.

 

[toolmaker96]

What is the maximum RPM for your machine, I suspect you need to be running flat out. In tool steel, we will be running 5500RRM & 40-45IPM. 5% radial or axial & running dry. Those #'s are probably conservative for the materials you list.

 

[mhajicek]

Max RPM on a Tormach is 10K.

When I've seen a Tormach cutting, it was struggling to slowly take a 0.100" x 0.100" cut in aluminum with a 1/2" endmill, and screeching like a banshee. They may be 30 taper, but they have the rigidity of a Dremel.

The correct answer is to sell the Tormach and buy a better machine. Failing that, I'd take the cutter manufacturer's feed and speed recommendations, halve the stepover and feedrate, and start there. Keeping the tool stickout to the absolute minimum possible will be critical.

 

[mmurray70]

Is the problem that 3/8 just doesn't provide enough material to keep the carbide from chipping?

Problem is the machine dont have enough material to keep the carbide from chipping.

You rpms and feeds seem too low. If your using a decent 3/8 4 flute variable helix try 6000 RPM and 36 IPM. Start with hardly any doc and increase doc until machine starts suffering. Probably wont be able to cut very deep.

Flimsy machines like the tormach will do much better with more modern adaptive type toolpaths.

 

[Wsurfer]

Carbide is very brittle and will not tolerate a floppy machine. Maybe try cobalt instead, and or a 1/4" end mill.

 

[trochoidalpath]

I have not had good luck with 3/8 inch carbide roughers in my Tormach.

I ran carbide roughers in my 1100S3 before I got a real mill. I did not have excessive wear issues in soft steels (unlike in 316).

If you can provide more info that would be helpful: stickout, LOC, depth and width of cut, what size ER holder are you using, what kind of tool path are you using…?

 

[bll230]

I'm with you on a real mill. I pride myself on not buying Chinese. However, I couldn't justify an extra $50,000 for a Haas and an extra $50,000 for the house to put it in for my model helicopters. My other machines are a 1956 Monarch 10EE, a 1947 SB heavy 10, an early 60's Clausing 8520, a 1942 Barber Colman #3 gear hobber, a 1971 Barber Colman 1-1/2 gear hobber, and a Boyar Schulz 6x12 surface grinder that was used at the BS factory and immaculate, 1960s(?). All rebuilt to like new. So I am a fan of American.

That said, this is what I was doing today. A specialized thrust washer, about 4 inch od, .4 thick, in O1 material. I was using a 3/8 carbide rougher to make the inner and outer reliefs, to then turn away the remaining material at the bottom to make my washer. I was using only 2500 RPM, .020 depth, 50% stopover, 10 ipm feed, 5 ipm plunge feed, and it did make the reliefs, but somewhere along the way the tips broke off. If not using carbide is the solution I will accept that.

I have Tormach 1100 series 3, stickout is about 1 inch, ER 25 holder, tool path for the circular part is circular. My max RPM is 5000

This is potentially helpful:

"take the cutter manufacturer's feed and speed recommendations, halve the stepover and feedrate, and start there. Keeping the tool stickout to the absolute minimum possible will be critical."

This as well. I can buy the add-on for Sprutcam.

"Flimsy machines like the tormach will do much better with more modern adaptive type toolpaths."

 

[trochoidalpath]

I hear you. Tormachs are nice in that there is a reasonable community around them and they fit in a lot of places that bigger mills won't.

Couple of thoughts about how I would make this part on a less-than-rigid mill. I have found that mill-to-mill differences on this type of machine makes "recipes" not as reliable as I would like.

1. Tool parameters for a Helical 59401 (HEV-C-5, 3/8" diameter, 0.020" corner rad): try 535 SFM (5500 RPM) and 0.0024 IPT (65 IPM), width of cut 0.035". This is derated pretty substantially for the tool.

2. You may have to play with the RPM and feed overrides to find a sweet spot but try changing the depth of cut. You do not have a lot of rigidity to work with. Tool deflection breaks edges.

3. Every time I have tried that sort of tool path (slotting around the outside) I hated it and myself. It was easier to just turn everything into chips starting from the outside. This way really helps with chip control and stops recutting, which is very hard on tools.

4. Similarly I would predrill the center hole to make entry easier.

Hope that helps?

 

[mhajicek]

Let's also look at which carbide endmill you're using. What brand and part number? There's a big difference between a generic eBay special and a high quality name brand material specific cutter.

 

[bll230]

TCPath- yes, very helpful. I don't use generic ebay. Garr, this Onsrud, Widia, etc. This endmill was an Onsrud 2 flute 81-842. They don't seem to make that exact 3/8 any more.

I'll get some Helicals and try as you suggest.

 

[BT Fabrication]

I'm with you on a real mill. I pride myself on not buying Chinese. However, I couldn't justify an extra $50,000 for a Haas and an extra $50,000 for the house to put it in for my model helicopters. My other machines are a 1956 Monarch 10EE, a 1947 SB heavy 10, an early 60's Clausing 8520, a 1942 Barber Colman #3 gear hobber, a 1971 Barber Colman 1-1/2 gear hobber, and a Boyar Schulz 6x12 surface grinder that was used at the BS factory and immaculate, 1960s(?). All rebuilt to like new. So I am a fan of American.

That said, this is what I was doing today. A specialized thrust washer, about 4 inch od, .4 thick, in O1 material. I was using a 3/8 carbide rougher to make the inner and outer reliefs, to then turn away the remaining material at the bottom to make my washer. I was using only 2500 RPM, .020 depth, 50% stopover, 10 ipm feed, 5 ipm plunge feed, and it did make the reliefs, but somewhere along the way the tips broke off. If not using carbide is the solution I will accept that.

I have Tormach 1100 series 3, stickout is about 1 inch, ER 25 holder, tool path for the circular part is circular. My max RPM is 5000

This is potentially helpful:

"take the cutter manufacturer's feed and speed recommendations, halve the stepover and feedrate, and start there. Keeping the tool stickout to the absolute minimum possible will be critical."

This as well. I can buy the add-on for Sprutcam.

"Flimsy machines like the tormach will do much better with more modern adaptive type toolpaths."


View attachment 343397

with this setup and design is tricky.

what is your order of operations on this part?
how are you holding this part? in a vice?
also as you cut, things move, id be a betting man the part is vibrating and moving and allowing it to chip the tooth off. inconsistant feed rates will kill carbide faster, and usually 90% is workholding. the other 10% is tooling and making sure its hard enough to cut the part, not all carbide is created equal.

id almost want to be having this laser or waterjet cut or a different process after the thickness is milled out.

 

[michiganbuck]

QT Wsurfer: [Carbide is very brittle and will not tolerate a floppy machine.]
or a floppy part or set-up.

If you tap a part with a small brass hammer and feel it resonate/vibrate, likely carbide cutters will be short-lived.

(grinding is the same, if you can move/distort a grinding set-up with two fingers the grinding action will be poor)

 

[bll230]

The stock was actually round, 1/2 inch thick to start. I was using 4 mitee bite t-slot clamps. Very secure, I think….

Good advice with the brass hammer tap.

 

[trochoidalpath]

I have not had great luck with the Mitee-bite slot clamps with a high depth of cut or a tall part. Too much force and the part can twist out or vibrate. They work pretty well for low profile parts though.

 

[michiganbuck]

A posting photo of your setup may be good. A mill fixture should be 1/2" construction or better to be solid at milling cutting forces. Even parts held in a vise can be up tipped off the vise floor and vibrate with milling.
*1/2" fixturing is light duty for milling.

A solid bolted down rail placed in the go direction that bumps/touches the part near its top edge held down with 1/2" T-bolts* (*more than one)...and Mitee-bite at the opposite might be better.

Heavy fixturing acts like a big anvil to not budge at each cutter slap.

Sometimes it is good to look at the cutting edge with a loop and at .02 (or what) wear-land, send the cutter to a sharpening shop for a .020(or what) grind/sharpening..

A mitee bite 3/8-16 screw as is found on a Mitee-bite is very light duty for a mill..that is why you most often you see 1/2" T bolts on a mill.

I have never used a Tormach so can't judge that machine. They look lighter duty than my mill, but they (Tormach) do have 1/2" T bolts. All the more reason for heavy fixtures.

 

[thesidetalker]

View attachment 343397

View attachment 343493

Wrong clamps. You're pushing the material sideways, not down, with those clamps. What do you think happens when you're profile cutting and you cut off the corners of the material? Clamp pushing the loose piece of material back into the cutter? Once loose enough, it's just going to bounce around... resulting in chipped tool.

In my experience, loose material left to do whatever it wants tends to result in broken shit.

Don't just leave chunks to "fall off". They're going to break things. Break tools, damage way covers, jam up augers/conveyors. Clamp it down or turn it into chips.

 

[Dalego]

machiningcloud.com If the tool manufacturer is listed and works with them a lot of the SFM is there. Adjust as needed. It is a very handy app.

 

[bll230]

Sidetalker, the actual stock was round so there weren’t loose pieces from the cut, but these later comments about the fixturing are well taken. This particular piece of round didn’t have enough rim to use holddowns when cutting outside. With this advice I probably should have milled out the center, using holddowns, and then used a disk with a stud through the middle to clamp the piece and remove the outer holddowns for the outer milling. All good advice.

 

[trochoidalpath]

I don’t like this approach because it makes it too easy to break concentricity. I would do this with a carrier; put it in Talon jaws, do the entire part from the top (drill through, inside profile to 0.010 over depth, outside profile to 0.010 over depth, etc) then flip it over, hold it in soft jaws, and take off the carrier. You have hit every surface but the bottom face in the first setup. Looking back in the thread I don’t immediately see dimensions on the part, but I would expect a 1/8” thick carrier to be OK unless this is bigger than I think.