Manufacturers recommended speeds and feeds seem way to fast

[Turbocharged]

So, I'm getting into running insert type carbide drills, and the recommended speeds/feeds just seem like they are just way too fast. I tried the recommended speeds/feeds on a bigger style (7/8) with a smaller holder, but it sounded awful (ear deafening squeal). I checked the hole afterwards and it looked good ... it was nice and smooth. Then I checked my insert for wear, and it still looked brand new. To get through my holes I ended just playing with the spindle speed switch and feed rate switch until the drill sounded half decent.

My question I guess is ... do I need to consider any other metrics? If so, can you list them and any associated formulas to help.

I'm going to guess that my holder length for my next drill may impact this but I'm unsure.

My Next Tool:

Drill: GEN3SYS® XT Series 11 (5XD)
Insert: C1 AM300 (7/16 dia)
Holder: Extended length (6 in projection) side lock holder
Materials to be cut: Nodular cast 200bhn & Grey cast 250bhn
Thru coolant: Yes
Fixturing: Extremely Rigid
Machine: Doosan nhp4000 horizontal

 

[boosted]

Squealing is often indicative that it wants more feed. It could have been lots of things though so who really knows.

One thing I can say for sure is that machinists are constantly overestimating the rigidity of their setup/workholding/machine; we are all guilty of it at some point.

If you are pushing a 7/8 insert drill, in relatively hard material, on a budget horizontal, with likely a standard CAT40 holder, do you really think that is extremely rigid?

 

[Turbocharged]

Squealing is often indicative that it wants more feed. It could have been lots of things though so who really knows.

One thing I can say for sure is that machinists are constantly overestimating the rigidity of their setup/workholding/machine; we are all guilty of it at some point.

If you are pushing a 7/8 insert drill, in relatively hard material, on a budget horizontal, with likely a standard CAT40 holder, do you really think that is extremely rigid?

The machine and tools leave much to be desired for rigidity... you are absolutely correct.... BUT the fixture on the other hand is very rigid no over estimation here.

 

[Mtndew]

You're only drilling a 7/16 hole in cast iron, it shouldn't be an ear deafening squeal.
That being said, indexable drills DO love to squeal, especially on a lathe.
What are the speeds and feeds that you're running it at?
I would start out at around 300sfpm, and feed at .0076 ipr and adjust from there.

Edit:
Are you using a 7/8 drill or a 7/16 drill? You mention both.

 

[MCritchley]

That squeal is the sound of money!
Carbide drills always make me nervous on the first few holes, as it’s typically quite fast. They like feed, follow what the vendor recommends.

 

[DouglasJRizzo]

In cast/gray iron the squealing usually indicates too light a feed rate per tooth.
Modern tooling is WAY beyond what most folk realize.
The Doosan NHP has a nice rigid spindle and TSC, so you may want to up the feed rate.
Go with what the tool maker says.

 

[PegroProX440]

I also get timid about running the manufacturers recommended speeds and feeds. Since most of my parts are one offs and some are pretty labor intensive, I don't want to jeopardize a failure. I can usually buy the tools I need for a job but not buy extras because I'm finding the sweet spot and breaking tools. So I just run everything conservatively. Let me know how it goes and hopefully I will grow a pair and send the drills harder.

 

[Mtndew]

I also get timid about running the manufacturers recommended speeds and feeds

Experience is the best teacher.

 

[Turbocharged]

I also get timid about running the manufacturers recommended speeds and feeds. Since most of my parts are one offs and some are pretty labor intensive, I don't want to jeopardize a failure. I can usually buy the tools I need for a job but not buy extras because I'm finding the sweet spot and breaking tools. So I just run everything conservatively. Let me know how it goes and hopefully I will grow a pair and send the drills harder.

Well... I decided to just send those drills into the part, and it worked perfectly.
First drill: 17/32 C1 AM300 Insert with a 5XD drill body. (2000RPM @ 20IPM) Spindle load was 12%
Second drill: 7/16 C1 AM300 Insert with a 5XD drill body. (2600RPM @ 21IPM) Spindle load was 11%

 

[TeachMePlease]

Experience is the best teacher.

Good judgement comes from experience.
Experience comes from bad judgement.

 

[MCritchley]

I also get timid about running the manufacturers recommended speeds and feeds. Since most of my parts are one offs and some are pretty labor intensive, I don't want to jeopardize a failure. I can usually buy the tools I need for a job but not buy extras because I'm finding the sweet spot and breaking tools. So I just run everything conservatively. Let me know how it goes and hopefully I will grow a pair and send the drills harder.

I’m in the same boat with some expensive one offs. For those I still use a hss drill that I know will work just fine. Yea it’s a bit slower and hole finish isn’t as good, but I know it will work fine and I might be just drilling a few holes in a part.

 

[RoundHouse M&F]

So, I'm getting into running insert type carbide drills, and the recommended speeds/feeds just seem like they are just way too fast. I tried the recommended speeds/feeds on a bigger style (7/8) with a smaller holder, but it sounded awful (ear deafening squeal). I checked the hole afterwards and it looked good ... it was nice and smooth. Then I checked my insert for wear, and it still looked brand new. To get through my holes I ended just playing with the spindle speed switch and feed rate switch until the drill sounded half decent.

My question I guess is ... do I need to consider any other metrics? If so, can you list them and any associated formulas to help.

I'm going to guess that my holder length for my next drill may impact this but I'm unsure.

My Next Tool:

Drill: GEN3SYS® XT Series 11 (5XD)
Insert: C1 AM300 (7/16 dia)
Holder: Extended length (6 in projection) side lock holder
Materials to be cut: Nodular cast 200bhn & Grey cast 250bhn
Thru coolant: Yes
Fixturing: Extremely Rigid
Machine: Doosan nhp4000 horizontal

sandvik 870 tip drills here in grey and ductile iron. ours ran 425 SFM and between .008-.018" IPR (1/2" drills normaly ran around .010"). grey always had a sequel and ductile was a more quiet squeal (if you could even call it that) with a smooth hiss. we used regular setscrew type endmill holders and majority of the time it was 3-5X diameter from 1/2" to 1.220" and all pilotless.

took forever to convince the boss this is what they sound like and it was normal, he was a firm believer in HSS drills only (not to say they dont have their purpose and are good for backups), but he couldn't get over how different they sound. but after the first year we had just about every diameter holder, going from 3 minutes on a set of holes to 20 seconds really helped.

The harder the grey the higher the pitch the squeal...... always (hated grey iron), ductile was always mild mannered and polite

 

[DMF_TomB]

So, I'm getting into running insert type carbide drills, and the recommended speeds/feeds just seem like they are just way too fast. I tried the recommended speeds/feeds on a bigger style (7/8) with a smaller holder, but it sounded awful (ear deafening squeal). I checked the hole afterwards and it looked good ... it was nice and smooth. Then I checked my insert for wear, and it still looked brand new. To get through my holes I ended just playing with the spindle speed switch and feed rate switch until the drill sounded half decent.

My question I guess is ... do I need to consider any other metrics? If so, can you list them and any associated formulas to help.

I'm going to guess that my holder length for my next drill may impact this but I'm unsure.

My Next Tool:

Drill: GEN3SYS® XT Series 11 (5XD)
Insert: C1 AM300 (7/16 dia)
Holder: Extended length (6 in projection) side lock holder
Materials to be cut: Nodular cast 200bhn & Grey cast 250bhn
Thru coolant: Yes
Fixturing: Extremely Rigid
Machine: Doosan nhp4000 horizontal

.
in my experience drill length and tool holder length effect vibration, thus
recommended feed and speed on short length drill on shallow hole and a
long length drill on a deep hole usually need different feeds and speeds.
if drill 10x dia in or 4.37" deep on .437 drill through coolant helps but might
not be enough pressure, i have seen tool coolant holes plugged before
especially if drill tip gets hot
.
i use a standard tool database (excel) that i list tool parameter like
dia, length of stockout, gage length, number of flutes, feed and speed, etc
thus a tool might have recorded 10 or more different feeds and speeds tried.
i list any sudden tool failures, and or reasons some feeds and speeds were
used. just saying after years or decades can easily not remember past
experiences. also even 1% failure rate or drill and or part lost 1 per 100 holes
is inconvenient. like driving a car maybe can drive 100 mph but chance of
severe car damage a lot higher than driving slower
.
sometimes cast iron might have hard spot or slag in metal and experience
random sudden tool failure. or drill breaking through other side might experience
random sudden failures cause tool is too close to max limits.
.
hole straightness sometimes can be off on high feeds, that is drill bends and
hole might be curved cause off high feeds