Using HSM on 304ss

[Dfrench]

I'm looking for some guidance on trying to get the best finish I can on some 304 ss parts. Machine cycle time at this point does not matter, I just need to produce one part with the best finish I can then go from there. I work at a quartz shop and I haven't had to cut stainless in a very long time. Cutting quartz we don't use the dynamic tool path whatsoever. So I'm not well versed on all of the options that dynamic toolpath entail. But I have been doing a lot of reading and research and think I have a grasp on most of it.

I have to make 50 of these parts that look like the holy grail from indiana jones on an older Okuma mill. They should be turned on a lathe but we don't have a metal CNC lathe. I have some destiny bullnosed 0.03" .5" diameter altin 4fl 1.5" loc end mills and I'm getting a real horrible finish. I'm starting with 2.52" round stock and the finish outer diameter is 2.5". Right now I just ran the outside convex and have not yet attempted the inside concave portion yet. I'm running 2d dynamic contour .02" stepover 500 sfm 0.001" fpt .433 doc with air blast leaving 0.01" for finishing then coming back and taking the whole cylinder portion in one pass. Looks like crap. Any help or insight would be greatly appreciated

 

 

Thanks

 

Frenchy

[crazy^millman]

Not trying to be mean here, but call up a local shop with a CNC Lathe and let them do this part. Trying to mill that is losing money IMHO.

 

I will try to offer some advise to help. You Stepover should be 10% min with 100% to 200% step down for the HST toolpath . I would also use a bigger diameter tool. That .500 diameter tool does not have enough rigidity to cut the material you are cutting. Might look to a 7 or even 9 flute tool for finishing in one pass with that chip load per tooth. For roughing I would kick it up to .003 to maybe .006 per tooth feed rate. On the concave section your step down needs to reflect a ball endmill representing the tool Radius you are using. Since you are using a .03R then you step down needs to be small enough to get a good finish. Again that small diameter tool is going to chatter having to stick out long enough and think for finishing you will find a bigger diameter tool to help achieve the results you are after. Crazy idea would be to make a form tool with that shape ground on it and then take a finish pass to machine it. Would have to be a good size tool and would be expensive, but I would again really consider farming these out to a CNC House with a lathe.

 

Sorry not much I can say to help.

[Matthew Hajicek - Singularity]

If you are going to surface with a bull, you might try using an up and down motion instead of along.  This will make the tool act like a ball mill larger than the bull it is, rather than the size of the corner radius as it would going along.

[Dfrench]

Your not being mean because this isn't anything that I haven't told the owner. These are stock parts that if I can make 50 we might sell 1-10 a year. The shop that has historically made these for us wants us to purchase a minimum of 100 at a time plus tooling and engineering fees. That would take us literally years to sell. She apparently has some other quotes out there but she wants to see if we can make these here. I told here we could but they would be ugly which is exactly what they look like.

We have a very small  metal shop that consists of a manual lathe and mill and a 15 year old Okuma 4020 that we use to make things for whatever the shop needs. This machine is not a production machine.  She doesn't care if we make a part a week as long as we have parts for potential orders. And right now we don't have any orders.

 

 

I am planning on using a 5/8" 5fl ball endmill for the concave side but I haven't got that far yet, the concave side will be mechanically ground after machining so finish there isn't nearly as critical as the aesthetic of the outside.

[balnh]

I would cut the 304 with coolant. I have better luck with juice than not on 304. Also I hear you on the making lathe parts on the mill sometimes you gotta make do with what you got.

[Colin Gilchrist]

The High Speed Toolpaths are for Roughing the material away from your part, with efficient material removal. They are not designed to finish any of the surfaces on your part.

 

You are better off machining the part, leaving .01-.03 excess material, then using a couple different paths to finish the part. For the "cylinder" portion, consider using a Contour Tool path, with one "rough" pass, and 1 or 2 finish passes. The final finish pass, I'd take .005 of material, with slightly lower SFM, and a very light chip load. (.0002 per tooth) The most important thing here is to use a different "finish" tool to make the finish passes. The Rough tool should remove the majority of the material, and will by definition, leave a rough finish.

 

For the "bell" portion, finish using the .03 CR bull endmill, but again, make sure this is the Finish tool. For machining the surface, try Surface Finish Flowline. Use a very small stepover (.001-.005 step over). And you should get a nice surface finish.

[Goldorak]

Find a shop with a CNC lathe, its a 5min cycle time to get those part done with a nearly mirror finish .... 

[Colin Gilchrist]

Also, have you considered a different finishing method? You might be surprised what can be accomplished with a buffing wheel, and some polishing compound. If you can get a perfect finish off the machine, that would be ideal, but sometimes you can find the "sweet spot", and save massive amounts of time with a little hand finishing...

[jlw™]

Buy a $90 ball turner on eBay and do it on the manual lathe.

[jlw™]

Also, is it cosmetic? If so why not use something like 303?

[Colin Gilchrist]

Hey, you've only got a few to make, and cycle time isn't an issue right?

 

You can get bar stock, and cut blanks slightly long on a bandsaw. Then get a large CAT 40 or CAT 50 collet holder (not sure what taper you've got), and mount the blank in the mill holder. Clamp some O.D. and I.D. lathe tools to your table, and use a Work Offset to treat each tool like a Gang tool block.

 

You can actually turn your VMC into a Lathe with some "outside the box" thinking. One of my mentors; Mike Slota, taught me that trick. He developed a process to make special ballistic test projectiles using his VMC as a Lathe, since we had to hold tighter tolerances than our crappy Lathe was capable of holding. It's not the most efficient way to do it, but it would work amazing for your application. Heck, you could rough the parts with your current process, and just leave .01 stock for finish. You could then hand write the finish program that "turns" the O.D. finish, and I.D. finish paths. You should only need two lathe tools.

[crazy^millman]

Hey, you've only got a few to make, and cycle time isn't an issue right?

 

You can get bar stock, and cut blanks slightly long on a bandsaw. Then get a large CAT 40 or CAT 50 collet holder (not sure what taper you've got), and mount the blank in the mill holder. Clamp some O.D. and I.D. lathe tools to your table, and use a Work Offset to treat each tool like a Gang tool block.

 

You can actually turn your VMC into a Lathe with some "outside the box" thinking. One of my mentors; Mike Slota, taught me that trick. He developed a process to make special ballistic test projectiles using his VMC as a Lathe, since we had to hold tighter tolerances than our crappy Lathe was capable of holding. It's not the most efficient way to do it, but it would work amazing for your application. Heck, you could rough the parts with your current process, and just leave .01 stock for finish. You could then hand write the finish program that "turns" the O.D. finish, and I.D. finish paths. You should only need two lathe tools.

 

Excellent idea and I have done it in a pinch. This might one of those times where thinking out of the box will be the best approach.

[Matthew Hajicek - Singularity]

I've done it too.  Didn't think of it this time.

[Goldorak]

its a good way to get a 12000rpm lathe for small parts  

[Matthew Hajicek - Singularity]

Automatic part changer too!

[jlw™]

ha, I didn't think about it either and I did it in my home shop a couple weekends ago.

[crazy^millman]

Automatic part changer too!

Yes sir load up your tool changer with parts and hit the green button.

[smckay1058]

Would Love to see a video of that in action!!!

[Dfrench]

Hey, you've only got a few to make, and cycle time isn't an issue right?

 

You can get bar stock, and cut blanks slightly long on a bandsaw. Then get a large CAT 40 or CAT 50 collet holder (not sure what taper you've got), and mount the blank in the mill holder. Clamp some O.D. and I.D. lathe tools to your table, and use a Work Offset to treat each tool like a Gang tool block.

 

You can actually turn your VMC into a Lathe with some "outside the box" thinking. One of my mentors; Mike Slota, taught me that trick. He developed a process to make special ballistic test projectiles using his VMC as a Lathe, since we had to hold tighter tolerances than our crappy Lathe was capable of holding. It's not the most efficient way to do it, but it would work amazing for your application. Heck, you could rough the parts with your current process, and just leave .01 stock for finish. You could then hand write the finish program that "turns" the O.D. finish, and I.D. finish paths. You should only need two lathe tools.

I think I'm going to give this a go and see what happens! Great idea, I'll try to post some pics 

 

Thanks guys for all your great ideas

[crazy^millman]

Simple 3D contour toolpath should do what you are after. Just need to draw your chain in the front view to get the motion you are after. Might require a little bit of post modification, but not to much.