# Does climb or conventional milling only apply to edges of the work piece?



## Pcmaker (Oct 14, 2019)

Does climb and conventional milling only apply when you're milling at the edge?

What if you're milling straight into the middle of a steel block?

I get very bad chatter/vibration if I climb mill, even in very small width of cuts, hence why I just don't do it.

I'm also getting chatter and vibration when I'm sometimes cutting my endmill right in the middle of a work piece even after messing with the speeds and slow feeding. Using 3/8 carbide mostly on steel with all the axis locked tightly, with the axis I'm using the only one that's not locked. Not sure what I'm doing wrong.

I'll take a video of it later on. I have a PM25mv mill


----------



## Cadillac (Oct 14, 2019)

It applies to everything not just side milling. One reason for chatter is when cutting a pocket the first cuts are using the sides and bottom of cutter. So the ratio of the cut is overloaded. I usually use the 50% modo. Using a .500 cutter I would only take .250 per pass maximum on a side mill operation. Doing a plunge cut I would raise the table as I’m traversing to easy the plunge. I only climb mill maybe for a finish cut if improves finish.


----------



## macardoso (Oct 14, 2019)

It doesn't apply to slotting cuts since the pulling/pushing forces on either side of the endmill tend to cancel out (more or less). Be aware however that cuts which have between 50-100% engagement (more than half the cutter diameter, but less than slotting) will still experience lateral forces due to climb or conventional cutting. The lateral forces are highest at 50% engagement and tend to diminish as you approach 0% or 100%.

If you get bad chatter when climb cutting, you might want to look at tightening up your backlash adjustment on your leadscrew. It is happening because your work is being pulled into the cutter.  

Also (from a G0704 owner), the PM25MV is not a big machine. If  you are trying to slot in steel with a 3/8" endmill, you're really pushing what this machine is comfortable doing.

Couple of tips:

Use a smaller endmill. I find I can push a 1/4" endmill happily in its operating limits, but don't have enough umph to drive the 3/8" (especially in steel)
Not sure if manual or cnc (assuming manual), but change your approach to removing material. If you need to hog out a ton of metal, drill it out first, then finish with an endmill.
The BLDC motor has low torque at low speeds. Use the backgear to get the motor running faster.
Use roughing endmills whenever possible. Their wavy flutes significantly reduce chatter and required horsepower.
Use of cutting fluids can aid in minor chatter problems
Make sure you are feeding hard enough. If your cutter rubs on the work, you will get chatter.


----------



## Pcmaker (Oct 14, 2019)

macardoso said:


> *Make sure you are feeding hard enough. If your cutter rubs on the work, you will get chatter.*



When I get chatter, I feed much slower. I guess I've been doing the opposite of what I've been supposed to be doing  which is feeding even faster

I guess I should start stocking up on 1/4" end mills also


----------



## macardoso (Oct 14, 2019)

Pcmaker said:


> When I get chatter, I feed much slower. I guess I've been doing the opposite of what I've been supposed to be doing which is feeding even faster



Without seeing/hearing the cut it is difficult to tell you 100% what is going on. When you are cutting, you want each tooth of your endmill to form a full chip. If you get dust or little needles, then you're cutting too lightly. The edge of each flute is not as sharp as you think it is. On a microscopic level, the edge is very blunt and you need to give it enough pressure to dig the edge into the material. If you don't, it will rub across the surface without cutting, creating heat, chatter, and tool wear. You may find that pushing a 3/8" cutting this hard will start to stall your spindle.

Also remember that these cutting forces can be on the order of thousands of pounds of force. Sometimes the machine won't be rigid enough for the cut you're trying to take no matter what you try. This is the point when you want to reevaluate your process.


----------



## Pcmaker (Oct 14, 2019)

Yeah' I've been getting little needles when I'm milling


----------



## Mitch Alsup (Oct 14, 2019)

When I mill a block of 6061 or mild steel, I arrange the cut such that the cutting edge is going into the surface being cut. This minimizes the bur created by the cutting, and makes post milling edge cleanup easier. 

With the cutter turning CW, as seen from above, the side facing the operator is traversed from R->L and the side facing the machine is traversed from L->R. This is a climb cut, Like you I tend to go slow (table movements) and cut slow (slow rotation speed). The slow table speed gives a very nice surface finish, and my cutters tend to last a very long time.


----------



## ThinWoodsman (Oct 14, 2019)

Mitch Alsup said:


> This is a climb cut, Like you I tend to go slow (table movements) and cut slow (slow rotation speed). The slow table speed gives a very nice surface finish, and my cutters tend to last a very long time.



What sort of RPM are we talking? For a half-inch cutter, are you doing 500 RPM or more like 300?
I prefer cutting slow and feeding slow (J-head BP in backgear), but when I do this with conventional milling I end up chipping cutters. Well, chipping the big cutters and breaking the small (1/4 and less) ones when they catch.


----------



## T Bredehoft (Oct 14, 2019)

When slotting, use a two flute end mill. Otherwise one flute is cutting across the face, one is cutting into the side at the same time due to flex of the cutter.


----------



## macardoso (Oct 14, 2019)

Pcmaker mentioned a 3/8" carbide endmill.  Lets look at values which "properly" engage the cutter and then lets try to boil that down to something a manual machinist might be able to use.

Since they post good cutting data for their tools, I will use a GARR Tool EDP# 13230 3/8" 4F uncoated carbide endmill used in 1000 series mild steel.
Surface Speed (SFM): 175
Chipload per flute: .0027"
Spindle Speed: ~1800
Slotting cut @ 0.375" depth
Feedrate: ~20in/min
Power required for cut: 2.75HP

Whoa! That's a lot of power needed

Let's reduce those parameters that down and try to get something around 600-700W (using the full capacity of the PM25MV)

Surface Speed (SFM): 80
Chipload per flute: .0015"
Spindle Speed: ~830
Slotting cut @ 0.375" depth
Feedrate: ~5in/min
Power required for cut: 0.70HP

So there is something you can actually do on this machine (this is full slotting in steel, 1xD depth of cut). At 1.5 thou chipload, you'll be getting real chips. I would be concerned that the cutting forces on this cut may be too much for the machine. A smaller tool would save you money on carbide and you can remove just as much material with it. Lower forces too.

So I threw out a lot of numbers, what does it all mean? If you need to make a slot through 2 inches of material, you would dial in around 830 rpm on the spindle and start feeding so that you finish the cut in around 25 seconds. Feed firmly and consistently and listen to the sound. A good cut should sound something like a hiss, no squeaking or screaming. If your machine can't do that with this cutter, try a smaller tool or a roughing endmill.


----------



## macardoso (Oct 14, 2019)

Links for the previous post:

Speeds and Feeds calculator: https://www.custompartnet.com/calculator/milling-speed-and-feed

Garr Tool EDP# 13230: https://www.garrtool.com/product-details/?EDP=13230

Open the imperial technical data link on that page for cutting ranges


----------



## Pcmaker (Oct 14, 2019)

Do you recommend using 1/4 endmills as the largest endmill I should use for my pm25?


I'm always worried I'll snap thinner endmills like 1/4" ones easier than I would 3/8" or higher.


----------



## macardoso (Oct 14, 2019)

Pcmaker said:


> Do you recommend using 1/4 endmills as the largest endmill I should use for my pm25?



Depends on the application. Since I do CNC, it is easy to program a 1/4" endmill to cut the radius of a larger endmill. On a manual machine this is much harder. Sometimes it is worthwhile to use the larger tool to do the job correctly.  

I was focusing on roughing out material and general cutting for my statements above (based on your comment of slotting). Finish cuts will use higher speeds and slower feeds more focus on finish than the type of chip coming off the tool.

My starting point for this size machine is 1/4" endmills (4F) for steel and 3/8" (3F) for aluminum. Adjust based on experience and needs from there.


----------



## Bob Korves (Oct 14, 2019)




----------



## Mitch Alsup (Oct 14, 2019)

ThinWoodsman said:


> What sort of RPM are we talking? For a half-inch cutter, are you doing 500 RPM or more like 300?



More like 220 RPMs.



> I prefer cutting slow and feeding slow (J-head BP in backgear), but when I do this with conventional milling I end up chipping cutters. Well, chipping the big cutters and breaking the small (1/4 and less) ones when they catch.



When milling harder stuff (from mild steel and harder), I chipped some good end mills before I realized what was causing the problem.
In my case, I was moving the table at the speed I would end up milling the part--this was chipping the cutter just when the cutter came in contact with the piece being worked. So, I slowly sneak up on the edge until it just scratches the surface, and then "present the tool" to the piece being worked so that I can feel the bending force in the handle being turned, done right you can feel the tool enter and bite into the work, and it is at that point where you can start moving the table at the anticipated speed. I have not lost a tooth or edge since I learned this (1.5 years:: except when I release the tension on the 1" carbide cutter and it fell out of the holder onto the table chipping one corner (grrrrr).)


----------



## stioc (Oct 14, 2019)

You can run any spindle speed you want for any cutter diameter you want. The thing that matters is the feed rate. Feed rate is easy to dial in if you have a CNC or auto-feed. I'm not sure how you'd do it manually though...for that it has to be based on the looks of the chips coming out (size, color etc). You can literally measure the chips.

Since I hate changing belts (and rarely do) and not having a VFD yet I still have to swap cutters from 1/4" to 1/2" with various flutes I use the following formula to figure out my feed rate:

feed rate=chipload x no. of flutes x RPM

Since 90% of the time my machine is set to 1060 RPM if I'm using a 1/4" 4 flute HSS endmill my feedrate will be:

feed rate = .001 x 4 x 1060 = 4.24 in/min

Chipload varies as well as feed rate calcs depending on side milling or slotting. There are some really good videos on YouTube, I think NYCCNC did a series and it was very well done. I highly recommend it even for manual machines just to get a better understanding of it.


----------



## Pcmaker (Oct 15, 2019)

This is a lot to take in


----------



## macardoso (Oct 15, 2019)

The truth is that unless you are doing CNC, you will work off of feel and sound alone. No math.

But... sometimes it is nice to see some real numbers to understand how fast or slow you should be cutting. 

Don't let us bog you down with the details!


----------



## stioc (Oct 15, 2019)

Agreed with @macardoso but don't be scared- the math is super simple. It's just three things you multiply together. This should allow you to be in the ballpark. In my example above 4.24 in/min is roughly 4/60= .06 in/sec you can check if that's what you're roughly feeding by doing one-Mississippi, two-Mississippi, three-Mississippi, four-Mississippi  and see if you milled/traveled approx 1/4". Doesn't have to be exact but as long as you're in the ballpark you should be good.

To answer your original question though, in slotting you're doing both climb and conventional so it doesn't matter where you start. This is assuming the slot is the same width as the diameter of the cutter. If you're just enlarging a slot then you're either doing climb or conventional (which is preferred in manual machines, except for the finishing pass). Of course the deeper the slot the more power and rigidity you'll need. Also slotting in alum can be a real pain because alum doesn't evacuate as well so fewer flutes is preferable and better to have aluminum specific endmills since the coating prevents aluminum from welding itself on to the cutter which will eventually break it if you keep feeding. So now you need air/coolant. Oh welcome to machining...we're here to help you (empty your pockets)  Just kidding...but if you have questions feel free to ask, I don't know a lot but I have experimented and broken enough endmills to offer advice based on my personal experience.


----------



## ThinWoodsman (Oct 15, 2019)

stioc said:


> Agreed with @macardoso but don't be scared- the math is super simple. It's just three things you multiply together



Part of the confusion is that chip load is something that you manage with the feed rate (as Mitch mentioned above), so using it to _calculate_ feed rate is a bit circular. I've come across more than a few discussions that provide something like the following:
  chip_load = feed_rate / (rpm * num_flutes)
  feed_rate = rpm * num_flutes * chip_load
Generally, one knows the number of flutes and the RPM, but that still leaves two variables to solve for. I suppose chip load might buried in Machinery's somewhere (away from shop so cannot check), but what would the general rule of thumb be? DOC * length (.005" cut on a 2" long surface = 0.010)?


----------



## macardoso (Oct 15, 2019)

Chip load is often recommended by tool manufacturers and can be extrapolated to those tools that are not provided with cutting data.

Chip thickness is determined by tool geometry, coolant method, and material properties of the workpiece.

Here is the chart by Garr Tool which I often reference. These chiploads are usable for both carbide and HSS, but the Surface Speed (SFM) is specifically for carbide.

Use the columns on the right, selecting your tool diameter at the top. When choosing cutting parameters, I usually start at the lowest end of this spectrum and step up from there. But again, I have a small machine and those using large equipment can push these numbers harder.

Chip load is usually thought of as independent of other cutting parameters. Chip load and Surface Speed (SFM) determine spindle speed and feed rate for a given tool. Then WOC and DOC are chosen based on the type of cut needed and available horsepower.

Try punching these numbers into a speeds and feeds calculator (https://www.custompartnet.com/calculator/milling-speed-and-feed) and see how they get you the cutting data you need. Try bumping numbers up and down to get a feel for what affects what.


----------



## stioc (Oct 15, 2019)

Great question and one that I struggled with early on. Chip load is something that comes from the endmill's manufacturer. It's the amount of material each flute is capable of removing per revolution. A 1/2" carbide endmill's flute will remove a bigger chip than a 1/4" HSS endmill. The same endmill will remove more material in 1018 steel vs. Stainless.  So the best place is to look at is the manufacturer's published data e.g. 
They will often also tell you a way to calculate it for slotting.


			https://www.the-carbide-end-mill-store.com/custom/uploaded/files/feedsandspeeds/Carbide_End_Mill_Feeds_And_Speeds_General_Purpose_AlTiN.pdf
		


However, for most of us hobbyists who are using 1/8-1/2" endmills in 1018 steel you want to make sure you don't go below .0005" per tooth as that will cause rubbing. I mostly use 1/4" and 3/8" HSS endmills and use .001" and .015" per tooth respectively. So you can write some of these down for your common end mills and tape them near the mill or make an index card and put in the calculator's pocket for quick reference.


----------



## Nutfarmer (Oct 15, 2019)

I was always taught not to climb cut with a manual mill. You will be quickly reminded not to when the part you are milling is thrown across the room. Have not used a lot of carbide mostly high speed steel. With the work most of us do just get the speed of the mill close or even a little slower and you  can tell the rest by feel and looking at the chips coming off.  We aren't in production. If it takes a second longer to make a cut and saves on the end mill i am happy. Where i end up in trouble is trying to hurry and burn up or break an end mill. All the math is great for production but you can bury  yourself in it real quick. You will have a feel for it after a while.usually if there are problems slower is the first thing to try.


----------



## Pcmaker (Oct 15, 2019)

Any tips on using a 1/8" end mill?


----------



## T Bredehoft (Oct 16, 2019)

Be gentle with it.


----------



## stioc (Oct 16, 2019)

Pcmaker said:


> Any tips on using a 1/8" end mill?



What's the job? what are you using it for?


----------



## Pcmaker (Oct 16, 2019)

I mean in general. I've already snapped 2  in the past. From what I've learned in this thread, I shouldn't slot DoC more than 50% of the endmill's diameter? 1/8 is .125, I think, so the maximum DoC slotting I should cut is .0625


----------



## stioc (Oct 16, 2019)

Several factors to consider especially when slotting. Since the WOC is constant the only thing you have to tune your cut with is with your speed/feed and the DOC.

The DOC for slotting with a 1/8" solid carbide endmill should be anywhere from .25 times the diameter to .05 times the diameter. Go here  http://niagaracutter.com/speedfeed scroll all the way down and see the footnotes on slotting and axial depth (DOC). Aluminum vs. steel vs. stainless etc will all require stepping up or stepping down on the feed/speeds. Start conservative.


----------



## Pcmaker (Oct 27, 2019)

Snapped my nice 1/4" 3 flute carbide endmill while side cutting hardened QCTP holder for my lathe. Had to use a 1/2" cobalt roughing endmill to finish the job

I'm gonna get a 3/8" cobalt roughing endmill and just use that for slotting and most everything else. I'll use regular end mill to do the finishing passes


----------

