[stabbs]

I bought these 1" endmills and these mini endmils from CDCO and I am getting alot of chatter when I try to cut mild steel.

I'm running a trial of GWizard to calculate the feeds and speeds. I tried running the 1" end mill at 450 RPM & 5.4 IPM cutting .01" with a .05 degree helical plunge. My machine practically starts bouncing up and down when it tries to cut. I tried changing the inserts and it sort-of helped. The finish looks like crap and its making my steppers miss steps.

I switched over to the .5" end mills cutting at 850 RPM & 5.1 IPM. This one cuts a little better but still isn't great. I cut down about .25" and started to get alot of chatter, like the end mill was bouncing off the side walls in the channel it was cutting.

I've never used these indexable mills and I do not have much experience cutting steel. What am I doing wrong?? :drowning:

[pete from TN]

capable of plunging? A lot of indexable carbide endmills are not.. Maybe you could drill a hole and then drop that endmill into the hole and then do your helical? What kind of machine is it? Peace

Pete

[stabbs]

Its a Cummins Geared Head Drill / Mill Machine 42827

I have it running right now and the z axis is visibly vibrating up and down. When I press down on the spindle the vibrations transfer to the xy beds.

[stabbs]

thanks for the response Pete. I believe you are right that they aren't capable of plunging. I tried the hss 4 flute it cuts very smoothly.

I know I am very green in machining and probably should have done more homework before purchasing, but shouldn't these be sold as fly cutters if they cannot plunge?

[photomankc]

You should be able to ramp a non-center cutting endmill in no?

[eartaker]

stabbs,

You should be able to tell you CAM program to plunge in an area off of the material or use a ramp feature. Also I would check to make sure your gibs are tight if you say it is "bouncing".

[digits]

It's a bit hard to see from those pics, but it looks like they take flat, triangular inserts. I had a problem with a similar indexable mill because the inserts were the wrong way round out of the packet. I chipped a few edges before I noticed and swapped them round - now I get excellent cutting results...

[gun_mike]

I think you may be going way to slow (rpm)

(CS x 3.82)/Dia

cutting speed for mild steel is in HSS is 100 sf/min general rule of thumb is to multiply by 3-4 for uncoated carbide tooling. so lets try 400

(400 x 3.82)1 =1,528rpm

Even 1,528rpm seems pretty slow. I usually run my 1" coromill 390 at 3000-3500rpm around 20-30ipm

for the feed rate you would be safe at .001-.002" per tooth, I wouldn't take anything less than that, as you will wear the cutting edge out prematurely.

From the link you provided I've gathered that they are two flute cutters. I also noticed, that in the photo there was no chip breaker on the insert. If you can, trying getting inserts with chip breakers, it makes a huge difference. Your feed rates should be calculated something like this.
CL x #Teeth x Rpm

.002 x 2 x 1528= 6.112IPM So your feed is good.

If I were you, I would try 1500-2000 rpm with coolant, and about 3-5 IPM.
remember to slow it down a bit (feed) for ramping in.

When using cam programs, you have to be cautious about how they produce feeds and speeds. You need to select the right material, the right cutting tool material, the number of teeth, and the chip load. I allways double check with the formulas, as they are usually rock solid. also sometimes your cutting tool manufacturer will provide you with recommended speeds and and chip loads for their type of cutter.

Hope this helps,
Mike

[stabbs]

Got some machining in this weekend and still having trouble with the 1/2" 1 flute end mills. I machined in from the side and made a few .05" passes at 1500 RPM (thats the fastest speed on my mill) 6ipm with coolant. The cuts were ok, but my whole machine was vibrating and it was very loud.

I also made the mistake of cutting in the wrong direction (climb milling?) This completely dulled an edge. I am going to order some new, hopefully better, inserts and maybe a good 1/2" roughing end mill.

for the feed rate you would be safe at .001-.002" per tooth, I wouldn't take anything less than that, as you will wear the cutting edge out prematurely.

Gun_Mike: Should I take cuts at only .001 - .002"? GWizard said to set the cut depth to .27". I backed this off to .125" at first and it was very scary. I thought even dropping it back to .05" was significant. Maybe I am trying to cut too deep?

It's a bit hard to see from those pics, but it looks like they take flat, triangular inserts. I had a problem with a similar indexable mill because the inserts were the wrong way round out of the packet. I chipped a few edges before I noticed and swapped them round - now I get excellent cutting results...

digits: would you have a picture showing the proper setup?

[gun_mike]

Gun_Mike: Should I take cuts at only .001 - .002"? GWizard said to set the cut depth to .27". I backed this off to .125" at first and it was very scary. I thought even dropping it back to .05" was significant. Maybe I am trying to cut too deep?

The Chip load of .001-.002" means that as each cutting edge passes through the material, its shaving off .001-.002".

What GWizard was referring two was depth of cut, how deep the cutter goes into the material. The max depth of cut for a regular end mill is usually half the diameter, so the maximum depth for a 1" Inch would be .5". However with indexable cutters, the max is the height of the insert.

Depth of cut (DOC) is specific to each machine and how rigid it is. I use machines at work that have the capability to take 1"+ depths of cuts. For a machine like yours, I would try with .05-.1". Steel can be very hard on benchtop machines.

Here is an image that depicts chip load, Its labeled as CT
http://cmailco.files.wordpress.com/2010/08/apt.jpg

Mike

[stabbs]

GWizard has the chip load set to .006 which seems too aggressive. Ill drop it down to .002 like you suggested, Mike and try again this week. Thanks so much for all your help so far!

[photomankc]

If you are trying to cut 0.050" a pass at 0.006" chip load in steel.... Yeah, that's aggressive on a benchtop mill. Carbide is generally not real sharp so the machine has to put some ass into it to cut. I would not personally run that DOC in steel. I'd back off to half that on DOC and chip load and work from there. In AL you could probably do that all day but steel is a whole other animal.


Sent from my iPod touch using Tapatalk

[mntn-biker]

Carbide likes it best when it is running hi-speed. Try increasing your spindle speed (and possibly reducing your feed rate) to see if this reduces your chatter. Ask the company where you bought the cutter and inserts from what they suggest for a good starting point.

[JMI80]

You are using pretty big diameter cutters with small machine! I don't use that big tools for steel even with 1200 kg small machining center
with 3,7kW spindle. With 3500-5000 kg VMC
1 inch cutter is OK!

I recommend you to try small diameter coated HSS or carbide rougher end mills instead of big one flute cutters.
Use rougher to machine extra material away and finish end mills only for finish operations.

Coated HSS rougher end mill could be good choice for your machine with 1500 RPM. Personally I use mainly Guhring cutters, so I can tell that they are very good, but something like Fraisa roughers or similar will also do good job.

Use only small diameter tools like 0.25-0.375 inch.
Benchtop machines can't take much.

Here's video of 150 kg heavily tuned benchtop mill
machining steel with 8 mm (~0.31 inch)solid carbide
rougher bought from Guhring:

YouTube - JMI80's Channel

If I remember right cut is 4mm (0.157 inch)wide
and 3mm(0.118 inch) deep. 4500 rpm, feed 900mm/ min
(35.4 inch/ min).

Here's video of 1200 kg light duty VMC roughing steel with same 8 mm (~0.31 inch)solid carbide
rougher:

YouTube - JMI80's Channel

First cut's are 17mm (0,67 inch) deep
and 1mm (~0.04 inch) wide. 4500 RPM, feed 800mm/ min(31.5 inch/ min). I would not try to use
much bigger than 8mm-10mm (0.315-0.393 inch)
cutters in steel with this 1200 kg machine.
Benchtop mill will fly to the moon and back with
one inch cutter !

[stabbs]

Aw man, JMI80, those videos really make me want a new mill! I'm cutting a 1/2" piece of mild steel right now with HSS taking .03" cuts at 2ipm. The piece I am cutting will take about 5 hours to complete. I bet with one of those mills you posted this same part could be cut out in about 10 minutes.

I had to put the carbide end mills aside - I am building a vice right now. Once thats finished Ill go back to playing with the inserts and tuning their speed.

[pete from TN]

That is a real pretty VMC ya got now, what brand and model is that thing? How do you like it? You obviously know what you are doing with the smaller machines, those videos you have made should be required viewing for anyone learning CNC... Nice work man... peace

Pete

[JMI80]

Aw man, JMI80, those videos really make me want a new mill! I'm cutting a 1/2" piece of mild steel right now with HSS taking .03" cuts at 2ipm. The piece I am cutting will take about 5 hours to complete. I bet with one of those mills you posted this same part could be cut out in about 10 minutes.

I had to put the carbide end mills aside - I am building a vice right now. Once thats finished Ill go back to playing with the inserts and tuning their speed.

You have't yet tried coated HSS roughing cutters?

Maybe you just need high performance cutter's
from good manufacturer instead of new machine? Naturally you can
get machine with more speed and RPM with lot's
of $$$, but after that you still need those high performance cutting tools!

Now with 1500 RPM machine you will manage with
reasonable priced good HSS finish and roughing cutters (20-50$ each),
but the with 4000-8000 RPM you will need solid carbide tools
when machining steel. Then your tool costs will also be 2-3 times
more.

With small 150 kg machine I usually use
maximum RPM recommend by tool manufacturer,
but I adjust depth and widht of cut
and feedrate according to machine rigidity and
horsepower. Usually what sounds good also cuts
well. Note that you will need some sort of coolant when cutting steel and aluminium with HSS. Mist coolant could be good solution if you don't have enclosure.

Many benchtop machinist's would be amazed
how much performance it is possible to get
out from small machine with good roughing cutters.

Buy milling cutters and drills from well known manufacturers
like Guhring, Fraisa, Secotools etc.
They have tool engineers that do R/D
and test cuts. Cheap cutters may look pretty similar, but there's differences in cutter flute geometry and big difference in performance and durability. It's OK to buy small benchtop machine, but it's NOT good idea to use bad low cost cutters. With small low rigidity and low horse power machine it's important to buy best milling cutters that money can buy.

[stabbs]

I purchased an hss end mill set from little machine shop when I first got my mill and they have been OK cutting plastics and aluminum as long as I take light cuts. I have been looking into getting some good end mills, maybe a .5" and .25" aluminum roughers to start. Thanks for posting the companies you prefer.

I bailed on milling my own vise for now. Its just taking way too long to cut steel. I prefer working in aluminum anyway, so will keep milling steel to very small parts.

JM- nice work on your mill. I took a look at your build thread and its way impressive! Thanks for posting

[digits]

I think my BF30 clone is a bit heavier than your mill stabbs, but with shallow DOC's I have had pretty reasonable results in mild steel with this 2.5" facemill. IIRC I was taking off about 0.25mm per pass, full width...



As for the triangular inserts, I don't really have a good picture - but here are a couple I do have:




That's my 40mm cutter in cast-iron. With the inserts in the wrong way, it wouldn't even remove the paint and scale from the iron - the giveaway was that the inserts wanted to walk out of the facemill. Once I worked out and flipped them front to back, it cut like the proverbial hot knife through butter...

[stabbs]

I have the inserts tapering outwards (towards the cutting direction). They seem to cut well, but I was trying to plunge with them.

What was your feed rate for both the mild steel and the cast iron, digits?