Conventional mill to remove taper???

[Larry1958]

I have been asked to change my programming methods from one of the machinist on the floor(imagine that). Anyway I have an Machinist on the floor that is insiting I change the way I program so that when rough milling to use the climb cutting approach, and finish using conventional. His reasoning is that this removes taper on the walls better. I have always programmed the CNC mills using climb milling mainly to obtain better tool life and get better finishes. I only conventional mill flame cut edges, or heat treated surfaces. I know on knee type manual mills it is prefered to conventional mill due to the flimsy ball screws but I have never heard that would be preferred on CNC mills. I would welcome any replies to this subject to see if this change should be made. Thanks in advance.

[Guest]

There are only a couple of reasons I would program any toolpath conventional.

 

That's NOT one of them.

 

If your endmill is cutting a taper, either it's too flimsy to complete the cut with out deflection or the endmill IS tapered. Either way changing direction is not going to change the taper.

 

JMO

[New Job]

+1 John

[3R!< W3NG3R]

+1 John

 

I learnt on manual machines with backlash (the kind you can see by eye) and the only reason to conventional mill was to avoid this. Tapers had nothing to do with it.

[Larry1958]

Thanks John,

 

I usually use a 2:1 method to figure the size tool to mill with. If I am side milling a 1.0" thick part I will not use less than a .500" end mill. This usually gives pretty good results as far as taper goes. If I need to have minimal taper I will take a spring cut, use carbide, or face mill the surface on a horizontal. Thanks John.

[Kevangel]

I learned as a Moldmaker cutting DEEP pockets in mold bases that "climb cutting" keeps endmill from gouging in corners or climbing into lower sections near tip. So climb cutting actually is more accurate if dun-rite.. maybe his cutters are dull or I have seen some new ones with taper. Its "metal safe" to climb cut. (manuel bridgeports you have to mill conventional unless you have bought "ball screws" and if you need to replace old screws, BUY ball screws from ball screw manufacturer)

[Guest]

It's funny you mention that Kevin, that's one of the few times I do conventional mill. Deep pockets to keep the tool from grabbing and jumping "into" the corner.

 

 

As far as tool type goes, is there something else besides carbide?

[Kevangel]

Actually I use climb cuts for pockets in Bridgeport to "finish" ,just snug lock screws and climb cut..I think ball screws are about same price for bridgeports (as factory original that ARE NOT ball screws)if you buy direct from manufacturer. (conventional cuts can allow high speed cutter to suck into part in corners) +1 or more for carbide.

[Müřlıń®]

A brand new 1.25 endmill with a 6" LOC can deflect a ton when climbing if one side of the pocket is open.

 

Sometimes you can wear out a brand new endmill just springing around a pocket in toolsteel.

 

The less passes around will be better if this is happening and only the guy at the machine knows.

I have had to spring around a pocket 20 times to take the deflection out and hold .001.

 

 

And I have actually taken the taper out by conventional just as your machinist on the floor is saying.

 

Sometimes it's the only way if you don't have several brand new cutters.

 

Nuthing wrong with climbing or conventional, I use both when called for. I do however try to climb whenever possible.

 

Murlin teh finess his deflection and his machinetool...

[Kevangel]

quote:

---

Sometimes you can wear out a brand new endmill just springing around a pocket in toolsteel.

---

If you use a dull or not real sharp end mill and on deep walls it starts lookin "shiney" you got problems (if your down to that last thou or so)...best to have brand new cutter right at finish...

[Müřlıń®]

Ya...I always used my new one for the finish and used the regrinds and dull ones for roughing.

 

I would make sure the taper was out for my fnish pass....

 

Sometimes though, even on just a P-20 moldbase, and using the correct speeds/feeds it would get shiny before you made it all the way around with a new HSS mill.

 

We started going to 7% cobalt and that hepled.

 

Then finally M2...

 

Then everyone found out what "fit" menat

 

But the government was a stickler about tolerances and even on stuff that didn't matter, they could hold you money.

[Kevangel]

quote:

---

We started going to 7% cobalt and that hepled

---

Yup, I forgot that...always buy cobalt as does not cost anymore when they re-grind cutter so well worth it...same for boring bars if you don't buy carbide, DO buy cobalt..

[within a thou]

If you want to resolve the issue don;t use a cutter with such a great LOC use one with a shorter LOC then reduce the shank by about .03 take multiple step down cuts at a higher feed to keep the cycle time the same and don;t program corners the same rad as your cutter open them up by .01 or so let the machine do a G03 instead of a straight G01 and there will be no chatter or biting in the corner at all

[The Iron Chef]

Hmm. this is really old school thinking with a grain of truth.

Kevangels first post does allude to a certain phenomenom that the "Machinist on the floor" talkrd about. that is:cut a heavy single pass slot in one direction only. The end mill "unwind" due to torsional stress. The outer corner of the cutter pulls in to the material more on the conventional side of a slot whereas the climb side pushes away. THink of it this way:

walk down the centerline of a snowey road. Keep your left foot pointed out to the left. Your right foot remains strait ahead as you walk. The resulant path would show a slight undercut on the left (direction of travel) wall of your path. the effect of the preceeding tooth of the cutter grabing a little and "unwinding". You would see the opposit effect with a left hand helix, left hand spiral cutter.

Completely uncontrollable to accuralty eliminate tapered walls.

 

 

-Keith from home

[kunfuzed]

That's funny you mentioned conventional cutting on a flame-cut part. Someone just sugested that yesterday on a part that was busting the inserts and consaquently destroying the insert holder. Why does this help?

[Kevangel]

Don't know about that but if a part is flame cut you need to have it "enough oversize" to get "under the hardened area" or have parts "normalized". What I do anyway..

[3R!< W3NG3R]

kunfuzed,

 

It's so your cutter doesn't hit the hard and abrasive skin. Instead the cutting edge comes from behind.

[kunfuzed]

Ohhhhhhhhhh.... makes perfect sense. Thanks!

[Eeyore-nonhuman forum member]

I have been asked to change my programming methods from one of the machinist on the floor(imagine that)

~~~~~~~~~~~~~~~~~~~~

ssssso What ?

He is from the low race creature ?

[Goldorak]

HSS= ford model T

 

carbide=ford GT

 

diamond coating= F1

 

here i NEVER use HSS end mills

 

ok carbide is more expensive but it's 10x faster

and i rarely had to make spring pass even with 4 or 6 inch deep !!

[Storkman]

quote:

---

And I have actually taken the taper out by conventional just as your machinist on the floor is saying.

---

+1 Murlin. We have done it here as well. And when using a form tool you can't shorten it up. Every method has a place.

 

I prefer to climb mill for tool life. But sometimes that isn't the biggest issue.

[Tarheel]

"Tapers had nothing to do with it."

I agree, Deflection from a dull cutter or too much feed will not decrease if you "conventional" mill instead of "climb" Mill.

 

Tell him he got out voted and to change to a sharp cutter- preferable Carbide and you won't have to worry about taper anymore.

 

Remember: Ideas are free- really good ones are rare. So, ideas, like opinions are subjective.

[Eeyore-nonhuman forum member]

Tapers had nothing to do with it

~~~~~~~~~~~~~~~~~

Wrong statement

The climb milling pulls part toward end mill while conventional pushes it in the opposite direction .

This tends to all sorts of tricks and features dealing with tapers ,thin walls and so on .

You need to see me milling the thin pipe 150 mm dia 1 mm wall thickness with 30 mm dia mill CONVENTIONAL

AND JUST TRY TO USE CLIMB MILLING .

But if it makes no difference to you - DIMM ?

[drago]

I have been asked to change my programming methods from one of the machinist on the floor(imagine that)

~~~~~~~~~~~~~~~~~~~~

ssssso What ?

He is from the low race creature ?

~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

 

Actually, while this machinist makes a good point,

 

a lot of them don't. A lot of them ask for things that don't make sense. I had guys ask me to stop putting comments in the program "cause it looks more uniform that way". I think he just didn't want anybody else to be able to run jobs he set-up, but who am i to question him.

[drago]

BTW i agree with you, eeyore. Conventional cutting does wonders SOMETIMES.