Thread: Hsm rules!!!

Originally Posted by PixMan

Why is the video gone?

Sorry about that. The content was kinda crappy. I deleted it, but added two good ones. The one titled "Production milling" is awesome.

Originally Posted by ToolPost

What was the condition of the tool after that shower of sparks at the break-through?

Is there a taper on the walls?

here it is after the 24 part run. the coating is slightly discolored but still running great. It is back in the "used, but good" drawer.

Here is the one that shows what I am trying to accomplish. If we are to take back our #1 spot in manufacturing, this is how we will have to run. I look at machining like a race car driver I know, "you never go fast enough" . This however is not at the expense of quality. I truly enjoy tool grinding, but the real reward is when a shop "sees the light", when it comes to alternate machining styles. I have seen owners faces lite up like a kid in a candy store. As an afterthought, I will post a video of steel castings (full of sand pockets) being machined with an uncoated carbide endmill. I am sure many shops have to deal with this problem.





Production milling - YouTube

I have been wanting to try the HSM type of slot cutting when the need arises. I'm wondering if there is a "rule of thumb" about the best/maximum tool diameter for a given slot width.

Originally Posted by kvom01

I have been wanting to try the HSM type of slot cutting when the need arises. I'm wondering if there is a "rule of thumb" about the best/maximum tool diameter for a given slot width.

Yes, is there a reason/benefit for selecting a 3/4" EM for the slotting instead of a ~1" EM like you used for the outside facing? Was a smaller diameter EM intentionally used for better chip evacuation or perhaps because that's the size tool you had on hand for the job with the shortest acceptable LOC; or are there other reasons?

Thanks for posting this James!

Originally Posted by kvom01

I have been wanting to try the HSM type of slot cutting when the need arises. I'm wondering if there is a "rule of thumb" about the best/maximum tool diameter for a given slot width.

My preference is the cutter be less than 1/2 of the slot width. You can go larger, but you will have to back off the amount of material taken each pass. I don't have any formulas, but someone on here should.

Originally Posted by kvom01

I have been wanting to try the HSM type of slot cutting when the need arises. I'm wondering if there is a "rule of thumb" about the best/maximum tool diameter for a given slot width.

70% of slot width or less is my preference.

Arc-engagement will depend on the material and length of cut.

And... as fast as trochoidal slotting may be, plunge milling is usually faster, when feasible.

Originally Posted by mbraddock

Yes, is there a reason/benefit for selecting a 3/4" EM for the slotting instead of a ~1" EM like you used for the outside facing? Was a smaller diameter EM intentionally used for better chip evacuation or perhaps because that's the size tool you had on hand for the job with the shortest acceptable LOC; or are there other reasons?

Thanks for posting this James!

I chose the 3/4 because of several reasons. The 30 degree helix creates less lift,great for minimum holding area. The 1" would have only been able to take about .010 per pass, the 3/4 was at .020 . Its all about angle of engagement. Also the larger endmill would have created more heat due to the low feed rate. slotting like this is great, but there is a lot of heat created because the radial cut is very light at the start and end of the cut. You are only getting true programmed rdoc at the center. Air blast would be a great help, for chip evacuation and cooling.

Smaller diameter tool means you get to spin it faster.
Since you have 4 teeth either way higher RPM gives higher feedrates.
At some point the smaller tools flexes and you have to back off chipload.
Average chipload is best calculated here in a CAD or software designed for light engagements as the standard formulas don't work.

Spend two or three days slogging though the parameters and I find when doing high DOC low radial engagment milling like this a 5/8 gives the highest MRR rates up to about 1.25-1.5 DOC. Deeper than this and a 3/4 is better because you need the thicker core for stiffness.

A good CAM system will program the correct feedrate when you are on the material and speed up to 1000+ IPM when you are in the air.

If you have never done it I'll warn you it is scary as heck when you first run an endmill 1 inch deep at 450 IPM.
Everything just looks wrong when the slides start moving and you will never get to the stop button in time if there is one small programming error.

You know you are getting somewhere when you start calculating your MRR in cubic inches per second on 4140.
Bob

One other thing to consider is wear on the ballscrew. When cutting a slot one axis does nothing but move back and forth. If the distance the axis moves is too small the lubrication can be pushed out of the area and ballscrew wear can take place. The larger the radius used when trochoidal milling a slot thats in line with x or y axis the better.

False brinelling is what Ed is talking about - there was a thread on emastercam last year somewhen about it. Quite interesting.
Apparantly by memory first 'discovered' by Ford when transporting cars on the railways - the cars would rock back and forth ever so slightly and when they got to their detination, wheel bearings were fooked.

I used 12mm coated carbide 3 flute in Robodrill and after slight tweaking we managed to cut trochoidal 15mm wide 20mm deep slot 1mm per second in low carbon construction steel. 4000 rpm, 800mm/min feed.
No vibrations, superior surface and chip evacuation was absolutely perfect.

I like HSM a lot. No way could I make this slot in conventional way in such a time in 30 taper mill in reasonable time and wear !

Table motions look so smooth and gentle, no sharp turns and accelerations.. like mother swinging a cradle..

Also - trochoidal will wear tool evenly. With conventional slotting, especially with 30 taper machine, you'll wear only 2mm end and also you get rid of corners very fast. Especially in steel.

Originally Posted by CarbideBob

Average chipload is best calculated here in a CAD or software designed for light engagements as the standard formulas don't work.

You can calculate back from the desired chip load easily enough. I find this typically puts me in the ballpark for testing at all stable modes.

IPT*D/2/(sqrrt(D*RDOC-RDOC^2))

where:

IPT = desired inch/tooth
D = tool diameter
RDOC = radial depth of cut

A 1/4" end mill at .010" RDOC and a desired IPT of .001", would need .00287 inch/tooth to achieve that.

I've found that many cutters --especially larger diameter-- can withstand a very large inch/tooth at which point you can throttle the tool for life, part output and/or finish. A little cost analysis is useful for determining which direction to go.