Kennametal Go-Drill

[neurosis]

Anyone used Kennametal Go-Drills?  

We just started an Inconel job that has some .1 X .45 slots that are about .28 deep.  We decided to drill the slots out before milling them.

We have about 125 of these parts and they have 4 slots each. We're drilling 4 holes in each slot prior to machining.  That means we have to drill close to 2000 holes in 625 Inconel.

I couldn't find the drill size I wanted with coolant through from Guhring so I decided to try one of these Go-Drills.  We've drilled 144 holes so far with the first drill and this drill still looks like its brand new.  For their budget line of drills, this thing is performing pretty well so far.

[gcode]

did you try MA Ford?
They make very good drills... lots of sizes and options and good prices too

[neurosis]

did you try MA Ford?
They make very good drills... lots of sizes and options and good prices too

I didn't think to look toward MA Ford.  We use some of their tools but I've never tried any of their drills.  I might have to check them out.  

We typically use Guhring for tougher materials and YG for about anything else. I decided to try these Kennametal drills because they were priced pretty well and we have a LOT of holes to drill.  So far I've been pleasantly surprised.

This same job has 6ea 10-32 STI threaded holes that we're having to thread mill.  I was expecting to get about 50 holes per thread mill.  I called Carmex and they suggested a rather expensive new tool that they make for hard metals parts. This things has blown through 50 holes without even making an adjustment.  I'm expecting to get a couple hundred holes per thread mill.

[gcode]

MA Ford's 3X Cyclone thru coolant drills are very good... and Made in the USA  :_thumbup:

[JParis]

We do use these GO Drills...

They definitely perform in our applications

[gcode]

This same job has 6ea 10-32 STI threaded holes that we're having to thread mill. I was expecting to get about 50 holes per thread mill. I called Carmex and they suggested a rather expensive new tool that they make for hard metals parts. This things has blown through 50 holes without even making an adjustment. I'm expecting to get a couple hundred holes per thread mill.

are these the Carmex HardCut thread mills?
they work really well..I like them because they cut top down, climb cutting.
I put big notes in the files warning of the M04 and G42 callouts.

Watch your thread depths with these
They work so well because there are three threads worth of cutter  and you are spiraling down
you are getting 2 spring passes with each cut so the machines diameter is very stable.
but... over time the first tooth will break down and your thread depth will get shallow

[neurosis]

re these the Carmex HardCut thread mills?
they work really well..I like them because they cut top day, climb cutting.
I put big notes in the files warning of the M04 and G42 callouts.

Watch your thread depths with these
They work so well because there are three threads worth of cutter and you are spiraling down
you are getting 2 spring passes with each cut so the machines diameter is very stable.
but... over time the first tooth will break down and your thread depth will get shallow

Yes, and Yes.

Thanks for the heads up.  We are threading the length of the three teeth below where we need to because we were worried about that.  50 holes in the thread gauge still hits the bottom no problem.  I suspect that may change as it wears.  

[MIL-TFP-41]

We use a ton of the GoDrills.
A few years ago we had a job, 718 inconel, 1/2" thick, with 1000 ea .098" holes thru them. I figured 100 holes per drill. We had 30 parts to make. So we needed 300 drills. No other vendor had the close to the inventory to do the job & even Kennametal only had 100 or so drills on the shelf. We were able to work out a deal with Kennametal to constantly turn around and recondition 50 of the drills to get the job done.
The GoDrill performed as good as their "performance" drill in that application.

[neurosis]

A few years ago we had a job, 718 inconel, 1/2" thick, with 1000 ea .098" holes thru them. I figured 100 holes per drill.

We're using a .0945 dia drill and only drilling about .3 deep.  We are up to 300 holes so far and counting with the same drill. Keeping my fingers crossed.  We have a few thousand holes to get through and don't have enough time to get these reconditioned.

[neurosis]

We're up to 560 holes now and I'm about to change this thing out just on principal.  We are going to shoot for 16 hours of lights out machining tonight so I'm going to load up anything that looks even remotely worn.  

The thread mill is on 216 holes and we've made one adjustment while it was breaking in. It's getting left in tonight with crossed fingers.

[gcode]

We're up to 560 holes now and I'm about to change this thing out just on principal.  We are going to shoot for 16 hours of lights out machining tonight so I'm going to load up anything that looks even remotely worn.  

The thread mill is on 216 holes and we've made one adjustment while it was breaking in. It's getting left in tonight with crossed fingers.

How did the lights out thread milling go?
What feeds and speeds are you running?

[neurosis]

How did the lights out thread milling go?
What feeds and speeds are you running?

We're on day 2 of 16 hours of lights out machining. Tonight will be 3 and if everything goes well, by Friday night we will have 64 hours of lights out on this order.  

On that particular drill we are running 70sfm and .001ipr  

We do have 1000 psi through spindle coolant pushing chips out but this crap is so gummy I ended up using G73 to allow it to break the chip so the drill doesn't end up with chips balled up on it.  I don't really like doing that with carbide drills but it's worked.

I can't say enough about the Carmex thread mills. They've far exceeded my expectations for 10-32 threads in Inconel.

[gcode]

Your feeds and speeds for the thread mill are what I was interested in
I've used then in inconel with good results but never even considered running them lights out
what tool holder are you using for the thread mill?

[neurosis]

The thread mill is running @100sfm and .0004ipt    S2513  F4.5ipm

I used their recommendations for this tool using their built in website software.  Apparently they were right on the money.  

We have it in an ER32 holder.  

The holes are only about .3 deep so that does help.   We aren't running a through coolant tool. They didn't (if I remember correctly) have this particular tool with through coolant.

[gcode]

You are correct, the HardCut line does not have a through coolant option