Sanity Check - Need help with feeds/speeds for 1in Spade Drill

Hello,

I have two questions, and was hoping someone would have some advice.

- 6061 Aluminum
- Haas VF4-SS with TSC
- Mounted to HRT-160 and 2x 5th Axis Picatinny Rail Mounts


You can probably guess what I'm making, but I need to drill a 1.000" hole 7 3/4in deep in 6061 Aluminum (later perhaps 7075). I have bought the bar and insert, and my machine is equipped with Through Spindle Coolant.

I suppose I'm a little nervous about this cut and was hoping someone could tell me if I'm crazy or not! (At least in concern to this one cut!) I am worried that my fixture isn't stiff enough, my machine not strong enough, or this cut too aggressive to accomplish my goals. I try to run my machine as conservatively as possible, since I own it myself and don't have a boss with a checkbook who will pay for mistakes.

I was thinking a starting at 600 SFM and .010 to .012 feed/rev. That translates to 2291 RPM and 22.9 IPM. Seems really fast to me. I am planning to plunge with no chip breaking.

Here is the tool:


Here is the part and fixture:


Datasheet for the tool:


Better image for my workholding (this isn't the correct orientation)


Am I overdoing it? It is highly desirable not to have to make another fixture as I plan to mass produce these, but is that necessary?

Thanks!

I would feel exactly the same way with that setup. Most of my experience is with manual machines and big drill bits that haven't been properly sharpened in years. Whenever I do CNC work I program on the low end for whatever the recommended speeds/feeds are and then I can always play with the manual overrides to speed up. I prefer that over programming fast and relying on slowing it down at the beginning and slowly creeping up to 100% programmed speeds/feeds.

You don't have any support in the direction the tool will be trying to push the part. My first thought is to do the following:

1. Orient the 4th axis to the vertical position (how it will be holding the part)
2. Toe clamp a sacrificial piece of material to the table below where the part will be held. Depending on tolerances you are looking for, you may want to face the top off of this while it is on the table. Make sure this piece is more than enough to account for how deep you have to drill through to get past the drill tip angle.
3. Place the bottom of the stock you are drilling through on the sacrificial piece and slide it over to be clamped to the 4th axis
4. Play with order of operations to get the part all the way down on the sacrificial piece and held to the 4th axis in such a way that it isn't tilted out of tolerance. Indicator on Z axis and run it up and down to check. A small angle to a part that tall would result in substantial location error at the bottom of the hole relative to the outside of the stock.

I'm sure lots of guys would do things different ways. This was the first thing that I came up with for this part with the information provided. In our shop I would do this on a lathe with a 4 jaw chuck. We don't have any machines with a 4th axis, but a solid 90 degree angle plate could do the same thing with a little more work clamping wise.

I've used an HRT-160 on a manual mill as a small turntable for some pretty heavy milling on an HBM and they are pretty stout. The connection between the fixture and your part is probably your weakest point. I think you should be fine with that setup so long as you don't overdo it. I'd drop the speed a little - run at the low end of recommended - and start at . 010" feed and see how it sounds. You want to be a little on the low end for speed anyway for deeper holes.

my experience with spade drills is run more conservative than recommended give mores consistent tool life
.
if chips have problem coming out of hole I have often seen drill bit end melted with part material stuck to it.
damage to part and drill bit and to machine is sometimes fairly quick or sudden.
.
if 10" drill depth at 10ipm feed, hole only going to take 1 minute. I have seen damage from 2% failure rate say
its often not worth it going 100% recommended feeds and speeds

If you are doing a lot of these get an aluminum insert from Allied.
Aluminum inserts are razor sharp and polished to keep it from sticking.
Your weak point will be the dovetails clamped in your vises.
If that is stable I would run as high as 8000 RPM and .015 IPR.
FWIW I run a 3/4" Iscar Sumocham with high pressure coolant in a VF2
at 5000 RPM and .01 IPR (I'm going fairly deep and not the best workholding). Spindle load is like 40%.
It's aluminum after all......

Well, I went for it yesterday and not super happy with the result. My spindle load peaked at 132% (not sure where, I had my hand on the e-stop and was nervously watching the part the whole time) and it didn't sound good. The floor shook and it just didn't "seem" healthy to me. To the point I won't try it again without changing things up.

Here is a video: (starts at 1:56)

Shared album - Alex Crane - Google Photos

Seems to start out good, but gets loud half way through.

2292 RPM @ 22.9 IPM (600 & .010)

Surface finish is meh.

Here are some of the chips I made, not sure if this is good for clues or not



The tool after:



Wondering if I need to replace my insert and try again, but firmly mounted to a vertical vice. It's just a bummer for workflow. I want to make 1000's of these over the next couple years.

Alex

Sounded fine to me on the way in. I'm not surprised it rattled a bit on the way out running that fast in aluminum. It's a long, relatively skinny drill, and the coefficient of friction between steel and aluminum is not super low. I would alter your program to either stop the spindle or greatly reduce the RPM on the way back out. And rapid out, don't dilly-dally about getting it out of there.

It definitely won't hurt to try the aluminum specific geometry if you don't already have it. I don't think you have a problem with workholding rigidity. Also, if you need a nice finish, use a different operation than drilling... Or get a drill specifically designed to provide the finish you're looking for.

I would bite the bullet and buy an Iscar Sumocham with a ICN drill geometry for aluminum.
Go with a 12xD drill and run it at 600 sfm and .008-.012 ipr.
Your chips should look like Nike checkmarks, not strips of aluminum.
I checked and Allied has no ALU geometry for the spade drills.

FWIW, Ingersoll and Tungaloy have the Sumocham equivalents, called Gold-Twist and Drill Meister, respectively.
They might be a tad cheaper than Iscar.

On edit:

I just read your first post again and saw you're only going 7.75" deep. 8xD should be fine and will be more stable.
The Allied coating appears to be either AlTiN or TiAlN. Neither is ideal for aluminum. The edges tend to build up and cause problems.

Just my $0.02.

Ran it again, changed RPM to ~2500 and IPM to ~12 (400 SCM .008 IPR) and it seems to work better, but still maxed at 126% spindle load. Talked to YG1 and they are recommending a different insert to reduce axial load. Will try it when it comes in, hopefully later today.

[video]https://photos.app.goo.gl/MYafJ7gWmRJ7azip7[/video]

Will report later with the results of the new insert.

Alex

Yes, please keep us posted. I am anxious to see how it works for you.

Tried the carbide insert from YG1, didn't work any better.

I'm wondering if my problem is chip evac, even with the thru coolant. I'm wondering what a good pecking strategy would be?

Here is my idea: (FEEL FREE TO OFFER CHANGES!)

1. Make a "pilot hole" by interpolating a 1/2 EM and go ~1" deep
2. Change to Spade Drill, rapid to 1" above part, rotate ~50 RPM
3. Slow plunge (12IPM) into pilot hole at 50 RPM, not engaging bottom of pilot hole
4. Spin up to 2500 RPM
5. Peck at 12 IPM retracting plunging to cut depth at rapids
6. After final plunge slow to 50 IPM and rapid out

Does this seem ok?
Next question is how to program for it.

Alex

The drill / insert combination is your problem.
Straight flute drills lend themselves best to horizontals or lathes.
The Allied spades work okay for banging out parts on the drill press or lathe
but they aren't really that great on a mill, especially going deep like you are.

Your coolant is fine. I have a Haas with 300 psi and it works just fine at 8xD.
Like I posted above, get an Iscar or a knock-off that has a head specifically for aluminum.

ChipSplitter,

I think you are right. My tool guy is working up some quotes for the Iscar. Looking at this:



It's dang near $800 and that doesn't even include the holder or the insert.

$800..??

That sounds REALLY high.
MSC should be able to beat that....
IIRC a .750 dia x 3xD body was $300 or less.

Just checked MSC's website.

Here is their part #: 02864742 $600 list.

Twist their arm for all it's worth and get them down to 500..

I believe those drills are not recommended to start a hole when using a body of that length. Maybe try starting with the same drill in a 5xD and coming back with the long one. Also consider going at it from both sides if you can get it to blend ok in the middle. As far as feeds and speeds I only have experience with the coated hss inserts but I would go about 250SFM and 0.010-0.012 IPR. Slower speed should (my own personal theory) make a cooler and chip that is less malleable and harder feed will help it break as well. If your load remains the same throughout the hole then chip evacuation is not your problem. If it is loading up towards the bottom then concern yourself with getting the chips out better. I'm not a fan of these drills personally so I'm a +1 for getting something else but I haven't tried a lot of what is out there besides Kenametal and that's most likely out of your price range. A shorter drill reaching from both sides should save you some money though. I haven't tried either of these and don't know the price but Mapal looks like a nice drill to me for what I assume is affordable. Iscar has a 3 flute insert drill that looks like a good performer as well. 3 flute may be the best choice for mostly aluminum. I would like to give both of these a try if I could justify them to purchasing. Haven't looked deeply into it but spade drills are on my list to find a replacement in the shop I work at.

Nagol said:

I believe those drills are not recommended to start a hole when using a body of that length. Maybe try starting with the same drill in a 5xD and coming back with the long one. Also consider going at it from both sides if you can get it to blend ok in the middle. As far as feeds and speeds I only have experience with the coated hss inserts but I would go about 250SFM and 0.010-0.012 IPR. Slower speed should (my own personal theory) make a cooler and chip that is less malleable and harder feed will help it break as well. If your load remains the same throughout the hole then chip evacuation is not your problem. If it is loading up towards the bottom then concern yourself with getting the chips out better. I'm not a fan of these drills personally so I'm a +1 for getting something else but I haven't tried a lot of what is out there besides Kenametal and that's most likely out of your price range. A shorter drill reaching from both sides should save you some money though. I haven't tried either of these and don't know the price but Mapal looks like a nice drill to me for what I assume is affordable. Iscar has a 3 flute insert drill that looks like a good performer as well. 3 flute may be the best choice for mostly aluminum. I would like to give both of these a try if I could justify them to purchasing. Haven't looked deeply into it but spade drills are on my list to find a replacement in the shop I work at.

Click to expand...

No, the 8xD is good for no pilot. You can do 12xD when you use the self centering HCP head. The 3 flute drill only goes to 5xD and they don't have an Alu geometry for it yet.
As for speeds and feeds, carbide will run insanely fast in aluminum. It's pretty much whatever is stable and productive (milling at 1500-3000 SFM).

Ordered the Sumocham 8D body and the aluminum head yesterday. Hopefully it we be here by Wed to try out. We are going to put it on a heat shrink holder and see how it goes. My tooling guy was able to get it $650 and $130ish for the head. Yes, it was cheaper on MSC but he has done a lot of work helping me with the research for this so of course I'm going to use him.

crane550 said:

Ordered the Sumocham 8D body and the aluminum head yesterday. Hopefully it we be here by Wed to try out. We are going to put it on a heat shrink holder and see how it goes. My tooling guy was able to get it $650 and $130ish for the head. Yes, it was cheaper on MSC but he has done a lot of work helping me with the research for this so of course I'm going to use him.

Click to expand...

Can't blame you at all for not getting it from MSC......
I buy from them if they have something no one else does or it's WAY cheaper.
I just mentioned them because I didn't know what distributors you use.