PDA

View Full Version : Climb vs conventional cut for slotting profile



beanbag
10-15-2011, 05:02 AM
I am using a CNC machine. Normally, I use climb milling whenever I can. However, there are a couple of times I need to cut a closed loop profile in sheet metal or plate and have the center section fall out. Usually it is the center section I want to keep. However, I have noticed that the conventional cut side has the better surface finish, while the climb side has the burrs.

Is there a rule of thumb for whether I cut the loop clockwise or CCW?

.RC.
10-15-2011, 05:40 AM
You have lost me..... You should not be using an endmill for slotting..

End mills are for cutting on an edge... Slot drills for cutting a slot...

It is climb milling for 50% of the time.

Jaakko Fagerlund
10-15-2011, 07:57 AM
You have lost me..... You should not be using an endmill for slotting..

End mills are for cutting on an edge... Slot drills for cutting a slot...

It is all climb milling when slotting...
I would advice taking a little update on end mills and what they can be used for and how, because what you said is not true.

.RC.
10-15-2011, 08:24 AM
really????

PixMan
10-15-2011, 08:27 AM
The term "slot drills" isn't very common in my area at all. I'd never even heard it until a couple of years ago. I think it's all semantics, because I've been using end mills of various types to mill slots for 30 years. I like the 3-flute ones especially. Call it an end mill, call it a slot drill, I don't care. Whatever it is, it works great.

DATo
10-15-2011, 08:28 AM
OK , this is just my opinion so take it for what it is worth to you. When cutting a slot in which the tool is buried in the material, (such as the sheet metal example you mentioned), the material on the other side of the conventional cut is forcing the cutter back against the surface you are machining if only for the exact moment it is removing the material at any one point, thus the tool is forced to remove the material. Imagine that you are cutting the edge of some piece of material that is hanging out the side of your mill vise using conventional milling; the cutter is meeting resistance and is pushing slightly away from the cut leaving residual material behind in its wake. Now imagine that you are pushing the cutter toward the material as it is cutting with a piece of steel from the "air" side of the cutter. The cutter cannot spring away so it removes all of the intended material. When a cutter is machining efficiently it will leave a reasonably good finish, but if it can "spring" away the bad finish you see remaining behind is nothing more than the residual material resulting from the "spring".

With a fairly thin piece of material where the cutter is not machining along the majority of its length you would probably be OK, but if you attempt to climb cut the ends of thicker pieces of steel or the ends of extrusions (all materials) you run the risk of having the cutter grab. When this happens you can gouge your material and/or break your cutter. This can be particularly nasty with large, horizontal cutters.

You describe your project as one which is made of thin material and as such I don't think it matters which direction you go. If the conventional side gives you a better finish then go for it. To my knowledge there is no hard and fast rule. The things I mention above I have learned are generally true through personal experience.

.RC.
10-15-2011, 08:44 AM
Sorry I was wrong in my first post...

When slotting as the cutter is in the work for 180 degrees of a rotation..

It is conventionally milling for 50% of the time and climb milling the other 50%...

beanbag
10-16-2011, 01:12 AM
Upon closer inspection, the climb side has the better vertical wall surface finish, however it is the side with burrs. This makes sense because the chip leaves the material on the climb cut side. Once I knock off the burr, the climb side actually does look smoother than the conventional side. So I think the rule of thumb is to still keep the climb side on the piece you want to keep.

macona
10-16-2011, 01:17 AM
Yeah, you got it. Climb milling gets the best finish. Everything I do has a climb finish cut. With conventional you can get chip welding which creates a rough finish.

lakeside53
10-16-2011, 02:37 AM
If I want a nice "burr free'ish" finish I try to cut the slot with a smaller-than-finish dimension endmill, then perform a "finish" climb cut around the edges. If I want, my mill has this as a mode - I can specify the size of the finish cut required. It will automatically arc-in/out the cutter when starting, changing directions or ending.

JoeFin
10-16-2011, 08:46 AM
I need to cut a closed loop profile in sheet metal or plate and have the center section fall out. Usually it is the center section I want to keep.

With thin sheet it is usually the "Rigidity" of the material that determins the finish.

I call this "Drop Out Machining" for lack of knowing the proper term. If the material is of sufficient thickness where I need a good finish on the edge I'll use a rough cut leaving 2 tabs 180 degree opposed and then use a finish cut of .050 or less taking out the tabs and allowing the finished part to fall out from the stock.

SGW
10-16-2011, 08:52 AM
My understanding is that what the Brits (and apparently the Aussies) call a "slot drill" is what we in the U.S. would call a two-flute end mill.

DATo gave a good explanation of the cutting forces involved. I originally saw a similar explanation in an article by either Tubal Cain or George H. Thomas, and it was a revelation.

Similar to Lakside53, to get a really good slot I'll make an initial pass with an undersize 2-flute end mill, then do a finish cut with a finish-size end mill.

firbikrhd1
10-16-2011, 12:01 PM
I believe the term "slot drill" is indeed a British term but with it comes some traditional meaning. Traditionally, a slot drill was two fluted and able to cut to the center on the end of the milling cutter. This enabled it to actually plunge into material as a drill. An end mill was originally the 4 flute type that did not cut to the center and if plunged would only go perhaps .030" before stopping (bottoming out on the non cutting area of the center). When the mill was raised a little "pip" of material was left standing in the center of the work.

These days perhaps "slot drills" with more than two flutes are available and advertised as center cutting end mills. Therefore the more modern difference between an end mill and slot drill depends not on how many flutes the cutter has but whether it will cut in the center and can be used to plunge as a drill.