1. ## Calculating Speeds/Feeds?

Looking for some help & guidance in determining the speeds & feeds for HSM tool paths. I found a reference to a HSM calculator but it's apparently unobtanium.

http://www.mmsonline.com/articles/le...o-the-handbook

Here's what I'm dealing with at the moment. I have a part with multiple small pockets to machine. The part is 303 stainless annealed. There are several 0.063" radius corners so a 1/8" endmill is called for. The pockets are open on the bottom. I have two options, I can cut the pockets with an 1/8" EM with 1/2" LOC and leave some extra on the wall on the second pass to prevent rubbing the shank then come back with a 1" LOC for a finish pass. Or I can use a 1" LOC and keep as much as possible in the collet and use it to machine the entire pocket. The thing that I'm most concerened about is tool deflection. I've already trashed a couple EM's and ruined one ER16 collet due to excess deflection.

What I'm using are 4FL TIALN EM's, the std. length is a variable flute and the ext. length is a finisher. The supplier calls for .0005 chip load and 375 SFM. I have 8000 RPM max on the spindle so that limits me to 262 SFM. That's for the std. length EM. Cat 40 ER16 holder 2.75" gage length. Initially I was running coolant but what I'm reading is that TIALN should be run dry in SS.

Looking for guidance on the feed rate, DOC, stepover.

2. ## Estimating Feed Rates

There are a number of issues.

Index your feed rate. For 303 use .004 x diameter x number of flutes x RPM.

Adjust your cubic inch per minute by square of the diameter of the tool. And by the inverse cube of the length less 1/2 the z depth of cut. new CIPM = old CIPM x (dia^5/(length - 1/2 depth)^3). The maximum value not to exceed new CIPM = old CIPM x dia^2.

To adjust for HSM, use this: new IPT = square root (old IPT x old CIPM / (w x d x nt x rpm)) w = width of cut, d = depth of cut, nt - number of flutes(teeth) and RPM your going to use. old CIPM = w x d x IPM or reference CIPM for your tool.

Start with .004 x 3 flutes x .2 depth x 1 (for a 1.000 cutter.) use the dia^5/(length - 1/2 z depth)^3 to adjust. As a starting point. new CIPM = old CIPM x new (dia^5/(length - 1/2 z depth)^3) / old (dia^5/(length - 1/2 z depth)^3)

Adjust your CIPM up or down accordingly. Down if you break a tool (70%) or up if it works 10% to 20% at a time.

Once you find what works best, you can then index it per tool dia and tool length accordingly. dia^5/length^3

3. Coolant or no coolant - follow the tool manufactures recommendations.

For finishing calculate per revolution NOT per flute. (Only per flute for end cutting using ground cutters.)

For an roughness average of 125 finish multiply the square root of the tool diameter by .0405 for periphery finishing. To adjust a feed to a better finish new ipm = old ipm x sqr(new finish/old finish). For RMS finish use .0382 as the multiplier.

Go back to the basics and if the radii are non negotiable so that a .125 will interpolate slightly--you MUST use .118 (MM) or .094 3 flute... That is the starting point and using the principles as stated above you will get back on track--not only on this particular job you are working on but it automaticialy gives you the key to others that you will do. What I am saying is that in the type of machining that you are doing on your machine that just as in chess--you MUST think positionally and not tactically. Keep in mind that many of the concepts of high speed machining are in fact FOLLOW THE MONEY.....and you will see why it has destroyed so many shops.... thanks (I simply do not know--and dont have the time to figure out the workings of this very great--but complex websight--as always anyone is free to contact me or put a personal message to my screename or Jeff Cuneo jeffhome10@att.net 954-806-1501--24-7 is fine. SR R+D machining and prototyping Motorola

5. Rustyolddo, G-Wizard does most of the calculations such as chip thinning and ballnose compensation mentioned in that article. You can participate in the beta test for free if you like:

http://www.cnccookbook.com/CCGWizard.html

Which CAM are you using to generate the high speed toolpaths?

Some things to consider:

- While you ultimately need a 1/8" EM to fit the corners, you should consider trying 2 tools. The first being a roughing pass with a larger diameter EM that is more rigid and can remove the material faster. Sure it can't get into those corners, but the 1/8" will do that on the later path. To do this conveniently you will want CAM with rest machining, but you can also get your CAM program to do this manually.

- Less width of cut will help reduce the deflection. Presumably your HSM CAM is creating toolpaths along these lines and already calculating feedrates adjusted for chip thinning.

- Be careful going too light on DOC or too slow on feedrate. You can reduce your effective chipload to the point where the tool is burnishing. In stainless that means work hardening and much shorter tool life. More here on that phenomenon: http://www.cnccookbook.com/CCChipThinning.htm

- 1" LOC for an 1/8" EM is asking a lot of it (think hanging a boring bar out 8 times its diameter, usally not happy from a chatter/deflection standpoint). I don't think I'd go there except for a finishing pass and even then only if the finish really required it versus multiple passes that are shallower. If you have to go that LOC, you have to scale back your feedrate and width of cut considerably. G-Wizard will offer some suggestions on that.

There are a lot of parameters to experiment with here. If you're making a bunch of these parts, it'll be worth it. Keep notes. If you aren't making many, err a bit towards conservatism and save the wear and tear.

Cheers,

BW

6. i dont feel like reading through a bunch of blabber so take this for what its worth.
1. indicate the tooth runout of the EM, on a 1/8 cutter you really need .0005 or less.
2. forget about all the HSM BS for for now, its all great in theory. But theory and the shop for need to meet somewhere in the middle.
Try 7000 rpm at 25ipm .06 Z depth of cut per pass .01 radial, id run coolant. put a .003 corner rad on each tip. More or less take a light lapping stone and in your hand go over the each corner 2 times. If this eliminates your chatter on roughing the corner out but it still chatters in the the last pass. You might want to try a smaller EM to finish the corner. Or if your tolerance allows it, try programming an additional .005-.01 rad in the corner so the EM doesnt Gouge into the corner as much