Recommended toolpath

[Thoob]

I have this part here that we cut quite a bit of. This style I mean. As of right now I use a High Speed Surface - area clearance to rough it out with a 1" high feed mill, then a flowline with a ballmill for finish. It works out to 1200SFM with .120/rev (3 teeth) with .6 stepover. So it basically gives me around the 10 cubic inch removal rate. I don't know if I should be using a different path. What do you guys suggest?

 

The highlighted surface

Part is 16" long by 7" wide. Diameter of surface is usually between 2.5" and 3"

[EX-wccprogrammer]

I have no idea of the scale, but if you run a lot of these, you might consider standing it up, drill and bore.

[Thoob]

Parts pretty long. 16" total. Usually they are the same length. The middle is 10.5" long.

[Newbeeee™]

Optirough?

[Guyinthedesert]

Optirough?

 

that's what I was thinkin

[EX-wccprogrammer]

If you have the travel, Big Kaiser has a twin bore that has the reach, and cuts aggressively even on interrupted cuts. It would reduce the time for this feature by 90% would be my guess.

[Thoob]

We have 28" travel on the Z. I don't think it would be enough. Anyway, Not really looking for extra tooling. I guess I should be more specific. We are not by any means a production shop so when I say we get these type parts a lot, I'm talking more like 6-12 parts per month if we're lucky. Sometimes go 6 months before seeing them. I'm just thinking of different toolpaths. What does the opti rough do that's different from the are clearance? I have not had a chance to ever try the opti rough.

[MotorCityMinion]

"What does the opti rough do that's different from the are clearance?"

 

It uses the full flute length of the tool. Think end mill. You also get to add the chip thinning factor and bump up the feed rate.

 

Program both paths and see the difference. What material?

[Thoob]

Its 44W Mild Steel. The thing is its a round surface, so you would never be able to use all the endmill surface. I'm using a high feed mill so the full length is .03"

[John Summers]

You could tip it up at 45 deg. and use an end mill with inserts. Cutter maintenance is easier than with a ball mill.

[Rotary Ninja]

Do a parallel toolpath going across the surface with a .030" or .060" Rad 5/8" Garr 5-Flute - One shot, like .100" stepover and 75 IPM leaving .030" material. Then a Flowline with a 3/4" Ball cutting along the surface.

 

What kind of cycle time are you getting?

[Thoob]

Its not a ballmill. Its a 1" high feed mill. I hog it out with that, then use a ballmill to finish it. The ballmill takes no time. Its the hogging out that does. I'm not really sure what you mean by tipping it up 45 degrees? What would I gain? I would end up with another set up and another operation.

[Thoob]

Do a parallel toolpath going across the surface with a .030" or .060" Rad 5/8" Garr 5-Flute - One shot, like .100" stepover and 75 IPM leaving .030" material. Then a Flowline with a 3/4" Ball cutting along the surface.

 

What kind of cycle time are you getting?

 

I actually have the whole part cycle here

Its 30 mins to get the whole thing done, minus the 8 holes which is about a min total as its an insert drill.

[TK-32™]

[Newbeeee™]

Doesn't look much wrong with that

[Thoob]

It looks ok yes, lol. But the removal rate is only 10 cubic inches/min. The 3/4" endmill you see is taking a lot more than that. However I appreciate the responses. I just wasn't sure if I was on the right type of toolpath or not for that type of concave surface.

[Newbeeee™]

Where's Rickster???- he makes mold plates so it would be good he he chipped in.

[RayD]

I'm a big fan of highfeed cutters, but they are not always the most optimal. Try Optirest (looking at a stock model) with step-ups turned on, Start at full Flute height and step-up the walls, I would set the step-up to the maximum material your finish tool can handle.

 

Essentially the same thing your doing now, but from the bottom up

[#Rekd™]

I would check out an AJX cutter.