Any suggestions? My first time HEM with MAsterCam!

[Metals and materials]

And I am trying High Efficiency Milling on Titanium hehehe. 

Using optirough. TOol is 6mm, 19mm LOC, 63mm OAL. 

Parameters are:  stepdown - .748 or 19mm ; steup: 15 mm; Stepover: 11% or .0259 in ; SFM: 210 which is spindle speed of 3395 ; feed rate of 12.22.

I am leading in as Profile Ramp

Any suggestions if I could do better. Attaching pics of part as well for better view. 

 

[crazy^millman]

Flute count? Tool Specific information would be helpful.

[Metals and materials]

4 FLutes. Carbide. Ball Nose endmill. it is a MON 63613 or MW21223001460B. Supplier's website is down and not showing up elsewhere. 

8 minutes ago, crazy^millman said:

Flute count? Tool Specific information would be helpful

 

 

[crazy^millman]

3 hours ago, Metals and materials said:

4 FLutes. Carbide. Ball Nose endmill. it is a MON 63613 or MW21223001460B. Supplier's website is down and not showing up elsewhere. 

 

 

Why only a ball endmill? Use a Bull Endmill to get most of the material out of it. Look to a 7 flute tool. Use the ball endmill where you need. A ball endmill by it's very nature will create more cutting force.

[Aaron Eberhard]

The first hit searching for MW21223001460B points to https://wsies.com/catalogue/product/2012553

which redirects to:  https://genericerrormessage.com/

HAH!

 

Either way, Yeah, Ron has the right idea.. Rough with a bull nose, which will keep it from center-cutting. 

[CNC CHRIS]

drill a hole so your bull end mill can plunge before machining. 

[Aaron Eberhard]

Any coatings?  That will have a big effect on cutting Ti. 

For what it's worth, HSM advisor is suggesting 7.5mm DOC w/ 4.8% stepover (.2856mm), 6650RPM 56.79 in/min (.0021 FPT/411SFM). 

Assuming (you know what they say...) 1.375" of stickout from the holder, at your DOC & WOC, it's saying there will be more than .0061" of tool deflection, which is a lot.  It's probably not going to sound too good

[Matthew Hajicek - Singularity]

You're going to want to finish those ribs with each stepdown of roughing; they won't be rigid enough to finish if you rough it all first.

[Newbeeee™]

5 hours ago, Matthew Hajicek - Singularity said:

You're going to want to finish those ribs with each stepdown of roughing; they won't be rigid enough to finish if you rough it all first.

"She gunna ring like a church bell DingDingDingDingDing".... 

[Aaron Eberhard]

10 hours ago, Matthew Hajicek - Singularity said:

You're going to want to finish those ribs with each stepdown of roughing; they won't be rigid enough to finish if you rough it all first.

Also, I'd recommend finishing with a reduced neck cutter, so you're not rubbing the entire flute length against those ribs.

[Jake L]

22 hours ago, Metals and materials said:

Any suggestions if I could do better. Attaching pics of part as well for better view. 

Agree with all the advise above. +1 to smaller stepover and more flutes.

My first reaction was 11% in ti is a lot, I was thinking 4-5% with a 5 or maybe a 7 flute EM.

If the pocket is only 1.237" deep I'd shoot for two .619" step downs instead of .748. No reason for the first step to be the full .748 and the second to be .489. Though Optirough may even out the step downs automatically?

[#Rekd™]

A lot of unknown's.......what machine? What is the tolerance/ surface finish requirements? Possibly it could be roughed and then finished with a sink edm (assuming the vibration on the mill is too much).

Hopefully this isn't a quoted job!!!!!!!

 

 

[Manofwar]

Something to note with the approach you're looking at. It's going to create a lot of straw like chips in the part that will be very hard to remove with flood coolant. If you have it use TSC, chip clearing can be a real nightmare on cavity work in Ti.

[Kyle F]

 

3 hours ago, Jake L said:

Agree with all the advise above. +1 to smaller stepover and more flutes.

My first reaction was 11% in ti is a lot, I was thinking 4-5% with a 5 or maybe a 7 flute EM.

If the pocket is only 1.237" deep I'd shoot for two .619" step downs instead of .748. No reason for the first step to be the full .748 and the second to be .489. Though Optirough may even out the step downs automatically?

 

Maybe it's because I mainly program for Haas mills, but I usually run 10% or less even on stainless haha. Now we are talking about a .236 dia endmill running at over 5x diameter stickout?? in titanium?! I'd be running probably 2-4 different roughing bull mills of varying diameters and stickouts to maximize rigidity.

I have also had INCREDIBLE results with helical high-feed mills. They have some with TPlus coating for harder materials.

https://www.helicaltool.com/products/high-feed-end-mills-steels-up-to-45-rc-metric-variable-pitch-coolant-through-reduced-neck

These are great and in their 6mm variety they have varying reaches of 12/24/36mm. It's hard to know without seeing a model or dimensions but if you're dead set on 6mm tool I'd be running one of each length, and as the tool stickouts increase your speeds and feeds should reduce to reflect that. The beauty of the high feed mills is that they love to run high stepover and low depth of cut, which is great for situations like this IMO.

They have their speed and feed chart on that page, use that.

When using the shorter mill, I'd run close to the top of the recommendations. ( 4% diameter depth of cut, as high of stepover that pleases you ) then as you move to tools that are further out start getting closer to that 2.5% diameter depth of cut.

They are bell shaped tools, so work really well on hard materials taking those light stepdowns. I personally would probably use typical 2D dynamic chains to get the majority of that roughed out, and then polish it off with a stock model + opti-rest to finish that curvature at the bottom of the I.D.

For finishing those fins, I would think of trying 2 ideas:

1) rough out the whole part and leave like .05 per side on each fin, and then finish ramp with a necked back low length of cut endmill (I'd personally run real low SFM and chip load here) I'm not sure how thick those fins are but sometimes the rigidity of that extra .100" below where you're cutting gives it enough strength.

2) if that doesn't work I would rough and finish them in steps like what was previously mentioned.

 

best of luck!! 

[Newbeeee™]

On 1/5/2024 at 4:14 PM, #Rekd™ said:

A lot of unknown's.......what machine? What is the tolerance/ surface finish requirements? Possibly it could be roughed and then finished with a sink edm (assuming the vibration on the mill is too much).

Hopefully this isn't a quoted job!!!!!!!

 

 

Hahahaha "No Bid"