High speed toolpath recommendations

[Roger]

I would like to remove the area in green with a high speed toolpath.  I've never tried any of these paths before, and would like some input.  I'm using Mastercam X6, the material is 304 SS, will be running it on a Haas VF5 SS.  The endmill I planned on using is a 1/2" 4 flute Widia Hanita TiAIN.  All replies, and suggestions are welcome.

BLANK.MCX-6

[CJep]

2D HSpeed peel mill

Be certain to use a good speed feed calculator that takes radial chip thinning into account, like FS Wizard.

 

http://zero-divide.net/index.php?page=fswizard 

[Roger]

I'll be giving this a try today.  Thank you.  I went to your link, (FS Wizard).  I didn't have much time to spend using the calculator, what should I be looking for with radial chip thinning?  As I said in my 1st post, never used any of the high speed tool paths before.  I've been using Mastercam since version 6, just never worked at a shop that could take advantage of these paths.

[CJep]

DOC is your depth of cut

WOC is your step over

Length is how much the tool is hanging out of the holder

 

If you plan to use more Highspeed toolpaths you are going to want to get familiar with that or another calculator.

With any tpath too slow of feed rate is as bad as too high.

The highspeed toolpaths allow you to run faster spindle speeds and higher feed rates than conventional tpaths, the sweet spot is a bit narrower.

[Roger]

Thanks!  Ran the 1st 2 parts with an endmill we ran on 210 parts yesterday, everything went fine.  My operator decided to switch it out for a brand new one.  BAM!  it snapped the endmill on the 3rd lead in.  I had him go back to the used one, and it's still going after 50+ parts.  I'm using your toolpath with the endmill running at 260 sfm .005 FPT.  What do you think?  To much bite on a new EM, I thought he might not have tighten it enough, except we use a torque wrench for this. 

[Roger]

A picture is worth a thousand words.

[CJep]

The step over in the sample file was 10%, you more than likely need to back it off between 5-8%

[Tim Johnson]

I don't have any 304sst speeds but our 316 speeds for a 1/2" Widia Hanita (TM5V0E13015BV) five flute are S3973 F132.43 @10% radial cut

and S4966 F341.78 @ 5%. You should be able to increase that 10% to 15% for 304sst.

[Roger]

Tim,  what is your DOC @ those speeds and feeds, and on what machine, tool holder?

[JonBlinder]

That's pretty close to what I run mine at. It should be able to handle full flute length depth of cut. 1.5 inches or so. That toolpath is designed to not put too much force on the cutter so it can handle the depth. If you're nervous the first couple times, try breaking it up to do .5 inch DOC or so. You'd be surprised to see what it can handle though. I run mine in either a solid holder or an ER collet holder. Just depends what I have setup or handy. There are some pretty good you tube videos of some HSM toolpaths too.

 

 

Sent from my iPhone using Tapatalk

[Tim Johnson]

Tim,  what is your DOC @ those speeds and feeds, and on what machine, tool holder?

 

Jon pretty much has it covered. The machines are 40 taper Enshu horizontals.

[chipman]

My go-to toolpath is Dynamic core.

 

A little bizarre when chaining but the toolpath will not engage in excessive material.

I have yet to snap any tools with it. (304 all day long)

 

+1 use the FS Wizard to get speeds and feeds, the things has never let me down when milling

 

BLANK_CHIP.MCX-6