Toolpath and operation recommendations on a part

laminar-flow · Jan 3, 2017

I have been running this part by machining as shown and cutting off the excess on the bandsaw. Is this a good method or should I be using a full depth HSM operation and machine all of the outside stock off? I'm just talking about the perimeter as the other operations to do the top surface and the ball mill profiling are about what they have to be.

Shawnrs · Jan 3, 2017

Rough it out with a facemill and then finish the profile with an endmill.

deljr15 · Jan 3, 2017

laminar-flow said:
I have been running this part by machining as shown and cutting off the excess on the bandsaw. Is this a good method or should I be using a full depth HSM operation and machine all of the outside stock off? I'm just talking about the perimeter as the other operations to do the top surface and the ball mill profiling are about what they have to be.

That looks like a perfect candidate for HSM.

Mtndew · Jan 3, 2017

HSM around the outer full d.o.c.
Flip it over and face it to thickness.
Done.

Finegrain · Jan 3, 2017

You're definitely doing it the hard way by plowing a groove around the profile. Poor endmill spends a lot of time buried. Run full axial depth with an HSM toolpath, 25-30% stepover.

Regards.

Mike

laminar-flow · Jan 3, 2017

That is what I thought. This part was programmed years ago and I was not that knowledgeable about HSM. I run about 6 every two years so it isn't that big a deal on this part. But thanks for the help. What RPM and feed with a 25% DOC? I'm only grabbing it on the bottom .125"

npolanosky · Jan 3, 2017

laminar-flow said:
That is what I thought. This part was programmed years ago and I was not that knowledgeable about HSM. I run about 6 every two years so it isn't that big a deal on this part. But thanks for the help. What RPM and feed with a 25% DOC? I'm only grabbing it on the bottom .125"

Tough question to answer without more information. What endmill are you using? How much stickout? What's you max machine RPM? How much horsepower do you have to work with?

Finegrain · Jan 3, 2017

Hmmm, not sure given that you're only clamping on 1/8". I use Talon Grips and am able to go 16,000 RPM x 25% stepover x 1" axial depth, with a 1/2" Diamondback. I find out PDQ if I didn't get an even grip with the Talon Grips :eek:

.

Regards.

Mike

laminar-flow · Jan 3, 2017

I have a TM1, 6K RPM max but running at 5K on this part, .5" 3 flue, max DOC 1.265 for a 1.25 finished part thickness. I'm using a 4" Kurt vise with 6" snap jaws. Yes, need to get some talons.

broke · Jan 3, 2017

HSM all day on that part. You're only making 6 so program it with conservative feed/speed. An extra 30 seconds of runtime per part is better than chipping a $50 cutter if it pulls out. You could also buy larger material and hold by more then go Gonzo on it.

SeymourDumore · Jan 3, 2017

OK, I'll be the asshole here...
Since when does an HSM toolpath ( ANY HSM toolpath ) beat a bandsaw for removing a .125" thick material?

Flow, I cut something extremely similar to this, approx 50 to 100 per batch multiple times a year. Starting with a 2 1/2" height, using a 3/4 3fl rougher
full buried, 4 passes.
Granted, it's on a geared VF, but 5000 RPM and 55 IPM makes very short time of the roughing, then a single pass with a 5/8 XL finisher.
Saw cut the excess is less than 20 seconds/ea.

In my view, HSM has it's place, but not on that part.

Finegrain · Jan 3, 2017

SeymourDumore said:
Since when does an HSM toolpath ( ANY HSM toolpath ) beat a bandsaw for removing a .125" thick material?

Saw cut the excess is less than 20 seconds/ea.

In 20 seconds you can turn 20 CI of 6061 into chips, so basically that entire piece of stock. For just the excess per the OP's example, an HSM toolpath has that disappeared in less time than it takes you to walk over to the bandsaw and back.

Regards.

Mike

SeymourDumore · Jan 3, 2017

Finegrain said:
In 20 seconds you can turn 20 CI of 6061 into chips,
Regards.

Mike

On a TM1 with 6000 max RPM you get an MRR of 60 CI ?

The number I've posted above yields approx 30, and the cutter leaves the material for a total of 4 secs.

I stand by my opinion, wouldn't even attempt HSM in my case ( not even in his 6 piece lot either )

Hazzert · Jan 3, 2017

Buy a round over tool and ditch the ball nose for surfacing and call it a wash in time HSM vs slotting.

1/8" is more than enough, full depth 6000 rpm, 100 ipm and keep speeding it up while watching the load meter.

laminar-flow · Jan 3, 2017

Lots of good info. What is a round over tool?

I use the .250 ball end mill for finishing the ramp up on the part, and the .062 radii which blends into the .062 corner round along the two level edges. Is that clear in the image?

I made some notes and when I do these again I will try HSM at full depth.

Hazzert · Jan 3, 2017

I actually missed the ramp on the part. So you can't ditch the ball nose entirely.

A round over tool is a profile tool used to cut a radius on a part allowing you to just contour the path in one pass. Only gotcha is every radii requires a different tool but they can be had cheaply for under $30 for the smaller sizes from sources like Harvey or even McMaster.

laminar-flow · Jan 3, 2017

Sounds like you mean, as we call it, a corner rounding tool. Yes, I have a bunch and use the .062 on this part.

G00 Proto · Jan 3, 2017

Since I have some experience with a similar mill (TM2P), I would go full depth with a 1.25" cutter. 6000 RPM, 65 IMP, 20% radial step over. I would leave .010" for a cleanup pass. Deck the top with a 2" 45 degree face mill leaving as little as possible on the surfacing, then step up and get the top surface. Surface with a .25" ball with a flowline surface finish at 49 IPM, then finish the OD with the 1/2" EM (to remove the burrs).

Flip in a soft jaw and ship.

It's a couple minute part with a TM mill.

laminar-flow · Jan 3, 2017

Not a 1.250 Ø cutter hopefully. I'm not sure what you mean about surface with a .250 ball. The part has two levels and a sloped curved surface to the upper level. The two levels have a .062 radii and the .250 ball blends the two .062 radii along the edged of the curved slope and also creates the curved slope while doing the .062 radii. Here is a better image and you can see the tool paths.

Mtndew · Jan 4, 2017

laminar-flow said:
That is what I thought. This part was programmed years ago and I was not that knowledgeable about HSM. I run about 6 every two years so it isn't that big a deal on this part. But thanks for the help. What RPM and feed with a 25% DOC? I'm only grabbing it on the bottom .125"

Don't let that 1/8" of holding stock fool you. That's what I use normally, and a lot of times those parts are 2"-3" thick, and 6" x 8"

Toolpath and operation recommendations on a part

Stainless

Attachments

Stainless

Cast Iron

Diamond

Diamond

Stainless

Cast Iron

Diamond

Stainless

Hot Rolled

Diamond

Diamond

Diamond

Stainless

Stainless

Stainless

Stainless

Hot Rolled

Stainless

Attachments

Diamond

Similar threads