Struggling with an awful o-ring groove

[JB7280]

I'm cutting an o-ring groove and I've tried a number of things without tons of luck.  I'm pretty sure in the design process, their goal was the opposite of machinability.  The o-ring groove is .135" wide, .078" deep, and .040" away from a 3" high wall!!!

 

I have a couple of custom endmills from Garr.  .1875" shank, .125" flute diameter, .100" flute length.  I wanted to have the biggest shank I can.  It's also got their diamond coating.  amorphous diamond i think.  Running it in a Lyndex, Cat50 VC6 holder.  Tool is 5.5" OAL, with 2.375" stuffed in the collet.   I thought the VC6 might be a good option because the collet is piloted at the end, so there is 2 points of contact.  I thought that might help a little with keeping the tool rigid.  I've tried all sorts of methods.   Full depth just wandered everywhere.  I expected that, but figured I'd try.  I've tried RPM from 3000 to 12000.  HSMAdvisor recommends .007DOC, 11300RPM, .0008ipt.  That was pretty noisy as well.  Does anyone have any suggestions to make this slot go a bit smoother?

 

The one thing I have going for me, is I don't have to ramp.  There is an area where I'm able to enter from the outside.  

 

[Leon82]

Tiny depth cuts with that much stick out. Also a shrink holder. Did you indicate the endmill in?

 

Can you get a good blend of you lay it down and use a tslot cutter?

[JB7280]

16 minutes ago, Leon82 said:

Tiny depth cuts with that much stick out. Also a shrink holder. Did you indicate the endmill in?

 

Can you get a good blend of you lay it down and use a tslot cutter?

No way to use a T-slot cutter, I didn't show the entire thing, but in other areas the o-ring groove has twists and turns.  

 

  I did indicate the endmill.  Wasn't able to get it perfect, but less than .001" TIR.  We don't have heat shrink, but I just might order one and shrink it with a torch.  Will I really see that much of a benefit over a good hydraulic, or solid, or other rigid type holder?  I've never used shrink, except for a homemade shrink drill extension I made once, lol...

 

 

[JParis]

Ramp cut the C/L very gingerly....then using a contour ramp, ramp it down .01 to .015 per pass, take a couple passes....your RPM will be in the 1k range with a feed of around 5IPM

Slow and easy is the only way

 

I get these kinds of things all too often

 

[JB7280]

20 minutes ago, JParis said:

Ramp cut the C/L very gingerly....then using a contour ramp, ramp it down .01 to .015 per pass, take a couple passes....your RPM will be in the 1k range with a feed of around 5IPM

Slow and easy is the only way

 

I get these kinds of things all too often

 

I don't have to ramp, because I can come in from the outside.  Are you saying it would be a benefit to ramp?

 

Right now I'm trying .005" depth cuts and it's WAY overcutting. 

[JParis]

1 minute ago, JB7280 said:

I don't have to ramp, because I can come in from the outside.  Are you saying it would be a benefit to ramp?

 

Right now I'm trying .005" depth cuts and it's WAY overcutting. 

Yeah, the down force cutting that included the Z to a point, helps stabilize the cutter.....if you just try side cutting, you will deal with deflection and getting sucked into the cut all day...

You "might" even try a conventional cut instead of climb milling....climb is great and most often the way to go but it can promote the cutter being sucked in..

[JB7280]

6 minutes ago, JParis said:

Yeah, the down force cutting that included the Z to a point, helps stabilize the cutter.....if you just try side cutting, you will deal with deflection and getting sucked into the cut all day...

You "might" even try a conventional cut instead of climb milling....climb is great and most often the way to go but it can promote the cutter being sucked in..

You say .010-.015" per pass.  This is a very long o-ring groove.  Not sure of the linear inches, but it's got to be at least 65" total. What ramp ANGLE do you think?

 

[JParis]

I wouldn't use an angle...

I simply do not worry about what it takes time wise to get some of these done, only that they get done right...

JM2C

[gcode]

could you do that area next to the wall with a small right angle head and a key slot cutter?

[#Rekd™]

Limiting the depth of cut like JP said…you might have to go down to 0.0005 per pass. 
 

You have to find the sweet spot for depth, speeds and feeds.

[JB7280]

9 minutes ago, gcode said:

could you do that area next to the wall with a small right angle head and a key slot cutter?

Pretty much the entire slot is next to a wall that is just as close, unfortunately.  

 

31 minutes ago, JParis said:

I wouldn't use an angle...

I simply do not worry about what it takes time wise to get some of these done, only that they get done right...

JM2C

I guess what I'm getting at, is if I'm ramping at .010" per pass, doesn't that make the ramp angle steeper if it's a shorter contour, and gentler if it's a longer contour?  So .010" per pass could be a wildly different cut, depending on the circumstances, or am I thinking about it wrong?

Just now, #Rekd™ said:

Limiting the depth of cut like JP said…you might have to go down to 0.0005 per pass. 
 

You have to find the sweet spot for depth, speeds and feeds.

The lowest RPM I tried was 3000, and JP suggested 1000 so I'm going to try lower like he said.  

[#Rekd™]

Do you have HSM advisor? It should give you some defection information.

[JParis]

2 minutes ago, JB7280 said:

I guess what I'm getting at, is if I'm ramping at .010" per pass, doesn't that make the ramp angle steeper if it's a shorter contour, and gentler if it's a longer contour?  So .010" per pass could be a wildly different cut, depending on the circumstances, or am I thinking about it wrong?

Yes and no...I concern myself more with not overcutting and stressing the cutter...on a larger/longer cut, I might increase that depth per pass....unfortunately, these are only "ballpark" suggestions....no 2 of these kinds of things seem to quite be the same for varying reasons. At the end of the day, it will take some trial and error to find that "sweet spot"

[Leon82]

Yeah I would start it out at .001 depth cut.

[JB7280]

1 minute ago, JParis said:

Yes and no...I concern myself more with not overcutting and stressing the cutter...on a larger/longer cut, I might increase that depth per pass....unfortunately, these are only "ballpark" suggestions....no 2 of these kinds of things seem to quite be the same for varying reasons. At the end of the day, it will take some trial and error to find that "sweet spot"

I'm going to start with your speeds/feeds recommendations, and try some different ramp depths.  Also looking into a heat shrink holder.  I have a friend at another shop who could shrink it for me, just to see if it makes a difference.  I'll update once I get it figured out, and let you know what worked.  Thank you.  

 

4 minutes ago, #Rekd™ said:

Do you have HSM advisor? It should give you some defection information.

I do.  Unfortunately it was pretty far off on this one.  HSM Advisor reported .0019" deflection at the parameters I'm currently running.  What I'm seeing in reality is more like .012"-.013".

[JParis]

One time I have to use a .031 endmill at 30x's length to dia ratio....we eventually got a cut that worked but it took so long to make a good one that engineering took it out and changed up hardware to make it easier to machine.

You're at 24x's...that's no easy thing...doable, yes, quick & easy, never.

 

Good Luck 

 

[JB7280]

2 minutes ago, JParis said:

One time I have to use a .031 endmill at 30x's length to dia ratio....we eventually got a cut that worked but it took so long to make a good one that engineering took it out and changed up hardware to make it easier to machine.

You're at 24x's...that's no easy thing...doable, yes, quick & easy, never.

 

Good Luck 

 

If you go by shank diameter I'm actually at 17ish xD, and that makes me feel just a little better.  

[#Rekd™]

21 minutes ago, JB7280 said:

I do.  Unfortunately it was pretty far off on this one.  HSM Advisor reported .0019" deflection at the parameters I'm currently running.  What I'm seeing in reality is more like .012"-.013".

When doing something this unknown I would go with 40-50% of the suggested speeds and feeds. 

[JB7280]

32 minutes ago, #Rekd™ said:

When doing something this unknown I would go with 40-50% of the suggested speeds and feeds. 

I'm going to give JP's suggested parameters a shot, and I've ordered a shrink-fit holder as well.  I've never used them, so I'm curious to see if it makes a difference.  

 

Do you find HSM advisor to be close even with oddball situations like this?  I find that for longer reach tools, HSMAdvisor starts to produce sketchy numbers.  No fault of HSMAdvisor, I think that's just an impossible thing to predict.  

[crazy^millman]

5 minutes ago, JB7280 said:

I'm going to give JP's suggested parameters a shot, and I've ordered a shrink-fit holder as well.  I've never used them, so I'm curious to see if it makes a difference.  

 

Do you find HSM advisor to be close even with oddball situations like this?  I find that for longer reach tools, HSMAdvisor starts to produce sketchy numbers.  No fault of HSMAdvisor, I think that's just an impossible thing to predict.  

Exactly and where some designers should be made to come out to the machine and make what they designed machinable. DFM(Design for Manufacturing) is sorely lacking and missing at the University level.

[#Rekd™]

9 minutes ago, JB7280 said:

Do you find HSM advisor to be close even with oddball situations like this?  I find that for longer reach tools, HSMAdvisor starts to produce sketchy numbers.  No fault of HSMAdvisor, I think that's just an impossible thing to predict.  

All you are looking for is a starting point and HSM Advisor is one piece of information. Then talking to the tool manufacturer is another piece. Then looking at your machine holder is another piece. Etc. As you already know this is a tough job.

Good luck! 

[JB7280]

8 minutes ago, crazy^millman said:

Exactly and where some designers should be made to come out to the machine and make what they designed machinable. DFM(Design for Manufacturing) is sorely lacking and missing at the University level.

Agreed.  We have have been working through a very large batch of new products for this customer.  Close to 100 new part numbers, all in various stages of their own design.  It's been frustrating, as many of the parts have lots of impossible to machine features.  Square corners, ridiculous L:D ratios, etc.  If there's a silver lining, it's that the massive group of engineers they have seems to be listening to what we tell them makes a part easier, or more difficult to machine.  Things like arbitrary weight saving pockets with tiny corner rads, etc, seem to be fewer and fewer.  

 

Hell, when I first started working on this part, which has lots and lots of keen-serts in it, they had them dimensioned as standard threads.  The engineers on the job had no idea that keensert's require a larger minor diameter, until I explained it to them.  

[crazy^millman]

4 minutes ago, JB7280 said:

Hell, when I first started working on this part, which has lots and lots of keen-serts in it, they had them dimensioned as standard threads.  The engineers on the job has no idea that keensert's require a larger minor diameter, until I explained it to them.  

That is exactly what I am talking about. How in the world with everything that we have at our fingertips on the Internet could ever design a part to use inserts and not know the hole needed to be bigger for the insert to go into???????? 

Basic common sense is not even registering here.

Sorry back to your 1st part of the question HSM Advisor is a awesome product and Edgar does good work. Yes it can be off in these situation because there are some many variables that go into the process hard to have a good idea what will work until you do some trail and error like others have mentioned in this tread.

[gcode]

12 minutes ago, crazy^millman said:

DFM(Design for Manufacturing) is sorely lacking and missing at the University level.

you and I both know it's missing at other levels as well 

[crazy^millman]

6 hours ago, gcode said:

you and I both know it's missing at other levels as well 

That is pretty much a given now a days. I am referring to the graduated folks with degrees that are worthless if this the kind of things they are not learning about manufacturing or willing to go investigate on their own. No one taught us this we applied some common sense and figured out that is I want an insert for a certain size bolt I need the extra room for that insert to fit into. Basic common sense to know this and design a part to be manufactured and not know that is just ignorant at levels it just blows my mind. You call out a seal what is the first thing a designer is supposed to do? Go look at the manufacturing specifications to machine the feature to work correctly in. Certain seals have certain tolerance requirements for machining the features they will work in. A Keensert is no different the designer needs look up what are the manufacturing specification for putting that into their design. Just lazy and entitled is what that screams to me.

Management in most companies not getting this I just roll my eyes and do what I need to get the work done. There is no excuse for any designer today to not know DFM and to get a degree some of these designers get and not be taught this is a disgrace to them and the places where they were taught.