[mls]

I have never machined much plastic before and now have a job that will require all .062 and .031 dia mills which I am not used to using.
The part is only .089 thick and is basicly just a square type cut out with a boss on one side all corners have a .015 radius.
My question is what to start speeds and feeds at.
Machine is mini mill 6k spindle I have carbide 2 and 4 flute mills I am thinking
that the 2 flute tools will be the way to go.

Thanks Mike

[makingchips]

Tool Diameter: .250

Number of Flutes: 2

Revolutions per Minute: 6000

Feedrate: 50 IPM

Axial Depth per Pass: .089

Radial Width of Cut: .250

Power Requirement: 0.3 HP

This will get you close.

MC

[makingchips]

Sorry I missed the .031 and .062

.031

Number of Flutes: 2

Revolutions per Minute: 6000

Feedrate: 9.5 IPM

Axial Depth per Pass: .016

Radial Width of Cut: .031

Power Requirement: N/A


.0625

Number of Flutes: 2

Revolutions per Minute: 6000

Feedrate: 19.2 IPM

Axial Depth per Pass: 0.031

Radial Width of Cut: 0.062

Power Requirement: N/A

As for drilling get a 135* split point screw machine drill.


MC

[mls]

Thank you MC I will start there at least these size tools are fairly cheap.
Thanks Mike

[makingchips]

Anytime. Let me know how you make out.


MC

[crabbass]

MC,
Are these numbers generated by a machining calculator?

[makingchips]

Yes, Granted I don’t ever run plastic but one of the calculators I have does have a wide Varity of plastic. Seeing no one answered his question I figured I would help the best I could. I plugged in his machine specs max rpm and material. It should get him close tweaking may be required.


MC

[behindpropeller]

What calculator were you using?

[makingchips]

X4

[extanker59]

Some of our parts are plastic. Delrin, Tecapro, and rydel.
We like HSS for the finish passes when possible. Lower RPMs than if cutting aluminum (plastic likes to melt). Conventional milling instead of climb makes better finish on walls. Plenty of coolant to flush. Deburr completely on the machine (using spot drill to break all possible edges). Onsrud makes some plastic cutting tools that work well too. (Don't work for them, just bought 4-6 tools)

[mls]

I have never used a machining calculator do they get you pretty close.
Are they on the conservative side or the max it will do entill failure.
Do they tell you basic power needed and does this ussually come in close.
Finally what one would you recommend and how much does it cost.
Thank You Mike

[crabbass]

Some of our parts are plastic. Delrin, Tecapro, and rydel.
We like HSS for the finish passes when possible. Lower RPMs than if cutting aluminum (plastic likes to melt). Conventional milling instead of climb makes better finish on walls. Plenty of coolant to flush. Deburr completely on the machine (using spot drill to break all possible edges). Onsrud makes some plastic cutting tools that work well too. (Don't work for them, just bought 4-6 tools)

If your machine produces a better finish when conventional cutting, it is probably due to something being loose.

[extanker59]

Our Haas VF-2ss is about a year old and cuts titanium and 17-4ph routinely with no problems. We talked to the supplier of the plastic when we were having issues of "hairs", burrs or poor surface finish. They recommended conventional milling. It works. Plastic is different.

[Mic6]

As mentioned before, Onsrud makes an Awesome cutter for this situation. I believe it's the Super O single flute series. Carbide, polished and razor sharp. We would climb cut .125 thick delrin and uhmw and these tools will leave a great finish and no hanging burrs(which uhmw likes to do). You'll still need to break the edge though. HTH

[Brepins]

We're running pvc now slot dim. .047+-.005 .125dp 1.5 lg... using .045 e.m. 3000rpm 3ipm z 3 steps...finish 6ipm work's great