How would you tackle this?

[metalmansteve]

I'm thinking I have to order a custom face groove tool.  Any other ideas?

 

Material is 49% cobalt.  

 

The order is for 1 each of about 7 similar parts.

 

Anode_shunt.SLDPRT

[jaydenn]

Trepanning tool. If you are clever, you can make one yourself... Buy a few insert cartridges and make the tube yourself.

 

J

 

[JoshC]

If you dont have a long enough lathe type tool for this I suppose you could probably turn everything except the slot and mill the slot. To me from what I see it looks like a smaller nice high feed mill with a ramping motion would be a good fit for that slot but again I am talking about milling so I don't know if that was an option or if your only looking to turn it.

 

They make some smaller sized High feed style mills that have some good reach so that is my thoughts but there are obviously other approaches that would work. then you would only be looking at finishing after that and a solid carbide should be easy to get with that reach and size, or if you are not making many of these and don't have the high feed mill I don't see why a nice solid carbide wouldn't hold up with the ramping motion even though it may not be as appropriate as a high feed mill.

 

I don't know what kind of tolerances your holding but the biggest advantage (in my opinion) of the lathe over the mill approach to me is you may have better taper control on the lathe whereas milling may deflect the tool some at the bottom so taper may be a little more difficult to work out if this part has some tight tolerances.

 

That's my $0.02 and I hope it helps

[crazy^millman]

On a live tooling lathe. I would C Axis mill the slot using Helix to ramp the material out of the face groove. I would then use 2 boring bars one turned to machine ID and one Turned to machine the OD. Now if it was a B Axis Lathe I would follow the same process, but I would use the one boring bar since I could just spin the tool in the B Axis and use it for both ID and OD work on that face groove. Might even think about roughing leaving stock for finish then pie jaw the part then put an expandable mandrel inside the part and then finish it the same way I mentioned above. Not sure if the Cobalt will stay stable enough with all the meat taken out. Since it is only one each and I have to assume the material is not cheap I would approach it with 4 operations on a Live tooling lathe. If I had a B axis lathe then it of course would be just one operation since I would do it the double transfer way. No MT can handle this and it requires to MT machine groups. Lathe freaks out also and would require to Lathe groups, but double transfer still allow you to finish the part in one setup of the machine if you approach it correctly.

[WestRiver]

ARNO face grooving tool they are premo for this type of application look them up on the web

[metalmansteve]

Thanks for the ideas.  I'll let you know my progress.  

[metalmansteve]

Ron, would you use the flat created by the end mill as the finish for the floor and the boring bars just for the walls?

[crazy^millman]

Ron, would you use the flat created by the end mill as the finish for the floor and the boring bars just for the walls?

 

Yes I would make sure to use a wiper style endmill that produces good floor finish, but I got away from Face Grooving tools when I could years ago. Trick is to lie to Mastercam for the finishing toolpaths using Lathe or MT. You must make a dummy toolpath to mimic what the milling tool has done. Other than that you are not only going to save a ton of money not getting face grooving tools and fighting the bad finish they will give you on the walls of that thin part you should also have everything you need in your shop to start on this part right away.

 

Did a part a couple month ago the face grooving tool was $650 for one tool. Process to face groove the part in aluminum was taking 22 minutes on the 2 Axis lathe. I did a time study to show them the difference using an endmill and we could have done it per part in 4 minutes. They need to produce 100 of these a month. Tools were cheaper and you save time doing it like I outlined. They didn't have a live tooling lathe and were okay doing it that way, but for me I see such a waste of time. One month that is costing them some real money and in one year you can see some substantial savings.

[JoshC]

Yes I would make sure to use a wiper style endmill that produces good floor finish, but I got away from Face Grooving tools when I could years ago. Trick is to lie to Mastercam for the finishing toolpaths using Lathe or MT. You must make a dummy toolpath to mimic what the milling tool has done. Other than that you are not only going to save a ton of money not getting face grooving tools and fighting the bad finish they will give you on the walls of that thin part you should also have everything you need in your shop to start on this part right away.

 

Did a part a couple month ago the face grooving tool was $650 for one tool. Process to face groove the part in aluminum was taking 22 minutes on the 2 Axis lathe. I did a time study to show them the difference using an endmill and we could have done it per part in 4 minutes. They need to produce 100 of these a month. Tools were cheaper and you save time doing it like I outlined. They didn't have a live tooling lathe and were okay doing it that way, but for me I see such a waste of time. One month that is costing them some real money and in one year you can see some substantial savings.

 

Nice, on a side note for some of you whom may not have seen this in a rollout, In 2017 Stock Models can now update Lathe stock using Milling operations. This was a stock model / lathe improvement that came with 2017's release and its pretty nice so you don't need to do the dummy toolpaths anymore.  Most may already be aware but if you weren't give it a try, its once of my fav enhancements other than the Dynamic Line of sight and lathe chip break enhancements

[crazy^millman]

Nice, on a side note for some of you whom may not have seen this in a rollout, In 2017 Stock Models can now update Lathe stock using Milling operations. This was a stock model / lathe improvement that came with 2017's release and its pretty nice so you don't need to do the dummy toolpaths anymore.  Most may already be aware but if you weren't give it a try, its once of my fav enhancements other than the Dynamic Line of sight and lathe chip break enhancements

 

Josh, that has no bearing on the lathe stock being used by Lathe and MT. If you want that to be aware you must use a dummy toolpath. Why does the software have us go through the process of defining a lathe stock if we must use a stock model to get the lathe stock to work correctly? If stock model is going to be the process then switch the whole part engine over to stock model and do away with gem of lathe which has been lathe stock so we can finally have it all work together.

[Müřlıń®]

49% COBALT........ouch!!  EDM/GRIND....

 

What kind of material has 50% cobalt???

[JoshC]

Josh, that has no bearing on the lathe stock being used by Lathe and MT. If you want that to be aware you must use a dummy toolpath. Why does the software have us go through the process of defining a lathe stock if we must use a stock model to get the lathe stock to work correctly? If stock model is going to be the process then switch the whole part engine over to stock model and do away with gem of lathe which has been lathe stock so we can finally have it all work together.

 

Hi Ron, I've been on these forums for a while now and know you certainly know your stuff when it comes to Mastercam so I was not trying to undermine your statements I just did not want newer users to Mastercam to assume you are required to make a dummy path since you no longer are required to do that in Lathe if you utilize a stock model correctly.  With that being said I do not have answers to your questions above nor do I know why the developers have the software setup in this manor but I will tell you that in Mastercam 2017 you can Mill a feature, Create a stock Model, then Turn that same feature and the Turning Toolpath is aware of the remaining stock due to the fact that a stock model was used. In x9 an Prior, this was not the case and your Dummy toolpath that you described was about the only way to get it done so I am just simply trying to mention that there is an alternative and easier way now.  From what I gather it sounds like you are saying that you wish Mastercam would not require a stock model or dummy toolpath to go from lathe Milling type ops to lathe turning type ops and I totally agree with you there. I also wish that was available and perhaps in the future but with how easy the stock model is to create in 2017 I like that we at least have that simple solution

[crazy^millman]

Hi Ron, I've been on these forums for a while now and know you certainly know your stuff when it comes to Mastercam so I was not trying to undermine your statements I just did not want newer users to Mastercam to assume you are required to make a dummy path since you no longer are required to do that in Lathe if you utilize a stock model correctly.  With that being said I do not have answers to your questions above nor do I know why the developers have the software setup in this manor but I will tell you that in Mastercam 2017 you can Mill a feature, Create a stock Model, then Turn that same feature and the Turning Toolpath is aware of the remaining stock due to the fact that a stock model was used. In x9 an Prior, this was not the case and your Dummy toolpath that you described was about the only way to get it done so I am just simply trying to mention that there is an alternative and easier way now.  From what I gather it sounds like you are saying that you wish Mastercam would not require a stock model or dummy toolpath to go from lathe Milling type ops to lathe turning type ops and I totally agree with you there. I also wish that was available and perhaps in the future but with how easy the stock model is to create in 2017 I like that we at least have that simple solution

 

Josh we are on the same page. Yes Stock model does support things much better in 2017.

[metalmansteve]

49% COBALT........ouch!!  EDM/GRIND....

 

What kind of material has 50% cobalt???

http://cartech.ides.com/datasheet.aspx?i=103&e=200&c=TechArt

[taperlength]

I'd use a Hougen to rough it out.  

 

http://www.hougen.com/cutters/magdrill/Hougen-Annular-Cutters.html

[Müřlıń®]

http://cartech.ides.com/datasheet.aspx?i=103&e=200&c=TechArt

 

 

Wow that stuff moves all over the place when heat treated...

 

Not too bad to machine when in the annealed state.

 

I assumed it would be alot harder...

 

[metalmansteve]

Wow that stuff moves all over the place when heat treated...

 

Not too bad to machine when in the annealed state.

 

I assumed it would be alot harder...

 

d.jpg

5-15% elongation when in thin strip form.  I have about 20 different parts to make.  Most of them are 5-8 inch rings x 1-2 inches thick.  These parts have to be annealed after machining for their magnetic properties.  I receive material that is hot forged from billet.  I'll probably anneal these before I even start on them and again after roughing....then again at final anneal.  If a .006 x 2.0 strip will elongate 5-15%....how do I calculate what an 8" ring will do without crazy simulation software?

 

I'd use a Hougen to rough it out.  

 

http://www.hougen.com/cutters/magdrill/Hougen-Annular-Cutters.html

 

This was my initial thought...even if I do end up milling it.

[Müřlıń®]

ok well elongation can be viewed 2 ways.

 

How much distortion the material is going to do during heat treat, and the other is based on the pull test up to breaking,

 

I think I was in error and the 5-15% on this chart is the breakage/ductility test.

 

 

 

But your question on how much the ring will shrink or expand during HT is a good question.

 

I think not much.  4140 has about 13% when tempered a certain way and usually .005/.01 per side stock on 4"ish parts will be enough to clean up critical bores and bosses.

 

But .006 thickness might be a whole different animal so I might want to do some research.

[Newbeeee™]

 If a .006 x 2.0 strip will elongate 5-15%....how do I calculate what an 8" ring will do without crazy simulation software?

 

Steve - unless I'm missing something, don't worry about elongation. It's only a ductility value to show how much it will linearly stretch (%) but within it's elastic limit.

So therefore it's a value that it will stretch, but then return to it's original length without permanent deformation. 

 

With your proposed heat treatments - I'd be more concerned about distortion through this and as they are forged billets, I'd have thought there's a huge amount of stress within the material.

But I haven't a clue what this stuff distorts like as never had to machine it.

Or wanted to machine it

 

Edit - I see The Mighty Morlin beat me with an answer - same time typing!

[metalmansteve]

Thanks guys!