Drilling inconel 718

[Bob W.]

I have a small inconel 718 casting where we will be machining around 300 pcs per month.  The machined casting has a threaded hole (7/16-14 3B) that is 0.900" deep and it is a through hole.  Halfway through this hole it is intersected by a 0.300" diameter hole that goes completely through.  The intersecting hols is perpendicular to the threaded hole and the axis intersect, so it is square to, and centered on the 7/16-14 hole.  My question is, what is the best method to drill this on a production basis?  We are using some Guhring 8510 drills right now but they are lasting eight parts (one cycle), so it isn't really cost effective.

 

Edit:  I should clarify, the 0.300" hole is cast into the part and we are drilling and threading the 7/16-14 hole.

 

[Guest]

9 minutes ago, Bob W. said:

I have a small inconel 718 casting where we will be machining around 300 pcs per month.  The machined casting has a threaded hole (7/16-14 3B) that is 0.900" deep and it is a through hole.  Halfway through this hole it is intersected by a 0.300" diameter hole that goes completely through.  The intersecting hols is perpendicular to the threaded hole and the axis intersect, so it is square to, and centered on the 7/16-14 hole.  My question is, what is the best method to drill this on a production basis?  We are using some Guhring 8510 drills right now but they are lasting eight parts (one cycle), so it isn't really cost effective.

 

Edit:  I should clarify, the 0.300" hole is cast into the part and we are drilling and threading the 7/16-14 hole.

 

You can buy cement drills real cheap and grind them to cut metal really nice, they are dirt cheap and have ceramic inserts

[Colin Gilchrist]

I'd go with a Replaceable Drill Tip, depending on how the Casting actually cuts.

Iscar makes a line called SUMOCHAM, that go down to 8 mm in size, and increment by 0.1mm increments. You'd need a 9.3 mm or 9.4 mm drill for a 7/16-14 Thread. About 100 SFM (may need to drop down to 60 SFM, based on the interrupted cut). This is the QCP-2M Geometry. Feed Chart shows 0.08 mm/rev, or about 0.003" per Rev., but that also may need to drop a little, based on the interrupted cut.

QCP 093-2M		9.30	3.83	1.970	136	9.0	IC908
QCP 094-2M		9.40	3.81	1.990	136	9.0	IC908

There is the part numbers for 9.3 & 9.4 mm sizes.

DCN 090-027-12R-3D

9.00

9.40

12.00

16.00

28.35

42.8

1.350

45.0

87.80

9.0

ICP 090

That is a drill body, with cylindrical shank, thru-coolant, 12mm connection size, 3.0-L/D ratio

Here is a 8mm Milling Cutter, with 1.5/1 L/D Ratio on cutting flutes > That is a .315-Dia Cutter (in.), with .709" of Flute Length, and 7-Teeth.

MM EC080H12R05CF-7T05

8.00

12.00

0.50

7

T05

7.70

18.00

36.0

3.0

0.03

0.10

IC908

[Bob W.]

10 minutes ago, Colin Gilchrist said:

I'd go with a Replaceable Drill Tip, depending on how the Casting actually cuts.

Iscar makes a line called SUMOCHAM, that go down to 8 mm in size, and increment by 0.1mm increments. You'd need a 9.3 mm or 9.4 mm drill for a 7/16-14 Thread. About 100 SFM (may need to drop down to 60 SFM, based on the interrupted cut). This is the QCP-2M Geometry. Feed Chart shows 0.08 mm/rev, or about 0.003" per Rev., but that also may need to drop a little, based on the interrupted cut.

QCP 093-2M		9.30	3.83	1.970	136	9.0	IC908
QCP 094-2M		9.40	3.81	1.990	136	9.0	IC908

There is the part numbers for 9.3 & 9.4 mm sizes.

DCN 090-027-12R-3D

9.00

9.40

12.00

16.00

28.35

42.8

1.350

45.0

87.80

9.0

ICP 090

That is a drill body, with cylindrical shank, thru-coolant, 12mm connection size, 3.0-L/D ratio

Here is a 8mm Milling Cutter, with 1.5/1 L/D Ratio on cutting flutes > That is a .315-Dia Cutter (in.), with .709" of Flute Length, and 7-Teeth.

MM EC080H12R05CF-7T05

8.00

12.00

0.50

7

T05

7.70

18.00

36.0

3.0

0.03

0.10

IC908

Thanks for the info.  The hole gets a threaded insert so the minor is 10.1mm.  If they offer in 0.1mm increments that would work great.  Any idea of the insert cost?

 

[CEMENTHEAD]

huge fan of ingersoll gold twist.  tips from: 6.0-25.9 mm

TD0900013S4R01 0.3543 0.3898 0.55 0.500 1.15 1.77 2.920 9 KTD6.0-D9.9

NEW-167-14_Gold-Twist.pdf

 

pro tip.. don't peck  inconel 718 . chip gets work hardened and will smash your insert on re-entry.

[crazy^millman]

Might be fighting some recast hardness at the cross section and might be at the threshold of what your going to get for tool life. Using replaceable tips was going to be my suggestion. Was doing some casting for one customer and every 4th hole we had to replace the drills. Might have got 6 holes per drill, but 4 holes was the accepted safe place and it was programmed accordingly. 30-50% of the total project anytime working with Inconel should be tooling cost.

Other thing might be going through the one section. Then come back and machine the next section flat then drill again. IF there is too much interruptions for the drill it will eat them up quickly.

[Colin Gilchrist]

1 hour ago, Bob W. said:

Thanks for the info.  The hole gets a threaded insert so the minor is 10.1mm.  If they offer in 0.1mm increments that would work great.  Any idea of the insert cost?

 

Unfortunately Bob, I don't know the cost on these. Those Ingersoll Gold Twist drills are also great. I used a 'replaceable tip endmill' from Ingersoll, (5-Flute, 1"-DIA, .250 Corner Radius), to replace a beast of a 2"-DIA Bull, with 0.25 Corner Rad. The company making the old 2" Dia. Cutter had stopped producing the tool, so even though this was a "locked process", we were allowed to substitute this new tool, "provided the part geometry during this Operation Step was not changed". (Had to produce the same part feature, even though the path was different, based on the tool size changing.

I'm used to paying anywhere between $40-150 "per drill tip", depending on brand, size, and application.

There are really two benefits when you go with the replaceable insert tip:

1. Tool Cost drops (typically), because you are only replacing a small amount of carbide, for a given insert
2. No changing Tool Length Offset. The inserts repeat to within about 0.001" of length, as the thread form is ground in the insert geometry. Plus, no removing the shank from the holder, means your Operator can judge the wear, and replace the tip at the machine while another tool is running. You should be seeing 0.008-0.010 of wear on that edge, where the edges are wearing, but not chipping or pitting. 

I'm with Ron though > back off 30% on the amount of wear you would normally permit on an insert, when you are pushing an insert cutting in Steel. Shoot for 60-70% tool life. Better to change out that insert 10 holes early, than 1 hole too late...

Since you need 10.1 mm, this also opens you up to Sandvik CoroDrill 880. These start at 10 mm Diameter, and go up in 0.1 mm increases as well...

[Colin Gilchrist]

49 minutes ago, CEMENTHEAD said:

huge fan of ingersoll gold twist.  tips from: 6.0-25.9 mm

TD0900013S4R01 0.3543 0.3898 0.55 0.500 1.15 1.77 2.920 9 KTD6.0-D9.9

NEW-167-14_Gold-Twist.pdf

 

pro tip.. don't peck  inconel 718 . chip gets work hardened and will smash your insert on re-entry.

This is also 100% true in 17-4 Stainless Steel. 17-4 work-hardens like crazy, so no pecking. Thru-Coolant, or increase your coolant Brix % (shooting for 12-14% concentration, watch your coolant ratio #, not all coolant mixtures are 1:1!), and don't peck or dwell.

[Bob W.]

41 minutes ago, crazy^millman said:

Might be fighting some recast hardness at the cross section and might be at the threshold of what your going to get for tool life. Using replaceable tips was going to be my suggestion. Was doing some casting for one customer and every 4th hole we had to replace the drills. Might have got 6 holes per drill, but 4 holes was the accepted safe place and it was programmed accordingly. 30-50% of the total project anytime working with Inconel should be tooling cost.

Other thing might be going through the one section. Then come back and machine the next section flat then drill again. IF there is too much interruptions for the drill it will eat them up quickly.

We have tried two strategies on this so far.  First we drilled completely through, straight shot at 1.5 ipm and the drill was chipped at the end.  Tool load went from 2.5% on the first hole to ~4% on the eighth hole.  The second strategy was to drill to center from both directions at 2.5 ipm (per reps interpretation of the chips) and the tool fared worse.  Chipping was worse and the tool load went from 3% to 6.25%.  We might have been able to get a second cycle with the first drill but it would have been risky.  No way would could we get a second cycle with the second strategy.  At $280 per drill this isn't feasible.  If an insert is ~$100 and we can get eight parts out of it that would be a process we can work with.  We have reached out to the Iscar rep to get some demo tools.  Thanks for the help on this.

[Aaron Eberhard]

38 minutes ago, Colin Gilchrist said:

This is also 100% true in 17-4 Stainless Steel. 17-4 work-hardens like crazy, so no pecking. Thru-Coolant, or increase your coolant Brix % (shooting for 12-14% concentration, watch your coolant ratio #, not all coolant mixtures are 1:1!), and don't peck or dwell.

I've gotten good drill life in 17-4 with no thru tool by just slowing down on the pecks, running ~50% rate from HSMAdvisor.  It seemed to avoid shocking the material so it didn't harden.  I think I was getting about 50-60 holes out of a ~.08" drill, which was quite acceptable for the equipment we had.  But it's certainly not max production!

[crazy^millman]

The casted .300 hole is your problem. Use a Highfeed cutter and plunge it first then come back and drill it. Drill life should go up exponential. Never chase a casted hole with a drill in Inconel. Mill it then drill it and think you will be happy with the results.

[AMCNitro]

Carbide insert drill, TSC and no pecking...

[Bob W.]

43 minutes ago, crazy^millman said:

The casted .300 hole is your problem. Use a Highfeed cutter and plunge it first then come back and drill it. Drill life should go up exponential. Never chase a casted hole with a drill in Inconel. Mill it then drill it and think you will be happy with the results.

We aren't chasing the 0.3" hole.  It is a preexisting (cast in) cross hole located halfway down the 7/16-14 hole we need to drill and thread mill.  We currently face the casting, spot drill with 142 degree spot drill, then drill with the 10.1mm carbide drill.  All is well until the drill reaches the 0.3" cross hole.  The interruption is killing the flute corners of the drill.

[crazy^millman]

12 minutes ago, Bob W. said:

We aren't chasing the 0.3" hole.  It is a preexisting (cast in) cross hole located halfway down the 7/16-14 hole we need to drill and thread mill.  We currently face the casting, spot drill with 142 degree spot drill, then drill with the 10.1mm carbide drill.  All is well until the drill reaches the 0.3" cross hole.  The interruption is killing the flute corners of the drill.

Might see about going to a Cobalt drill and running 10-12 sfm and see how long they hold up. With a good coating it might surprise you. I might try a sintered or compressed material drill. Sometimes slowing down the drilling actually speeds things up in a situation like this.

Have you tried using a 10mm 2 Flute Endmill to plunge the hole? Drill to just before the cast. The plunge with the endmill past it then bring the drill back and finish to depth. I would tell the customer to remove the stupid cast hole from the part. It cannot be helping anything and seems to be hurting more than whatever it is meant to be doing.

[Guest]

18 minutes ago, Bob W. said:

We aren't chasing the 0.3" hole.  It is a preexisting (cast in) cross hole located halfway down the 7/16-14 hole we need to drill and thread mill.  We currently face the casting, spot drill with 142 degree spot drill, then drill with the 10.1mm carbide drill.  All is well until the drill reaches the 0.3" cross hole.  The interruption is killing the flute corners of the drill.

A disposable drill like the cement drills would be perfect I think, you would just need a carbide grinder in the shop and you could redress it when the corner wears, I used to use them to remove broken hardened pieces of tool steel like d2 from molds, they only cost a few dollars so it doesn't matter if they break, but they usually need to be ground with some clearance, at least the ones I used did.

You could deploy it as a secondary tool only for the bad area with the cross

[JParis]

59 minutes ago, Bob W. said:

All is well until the drill reaches the 0.3" cross hole.  The interruption is killing the flute corners of the drill.

What I've done in the past is drill to just shy of the crossover..then mill past the crossover and repick up drill after the crossover

[neurosis]

14 minutes ago, JParis said:

What I've done in the past is drill to just shy of the crossover..then mill past the crossover and repick up drill after the crossover

That's what I would suggest if it's possible.

Drilling through a cast cross hole in 718. 

 

[Newbeeee™]

On 2/15/2022 at 10:43 PM, JParis said:

What I've done in the past is drill to just shy of the crossover..then mill past the crossover and repick up drill after the crossover

This. 

Drill to nearly break through, then spiral ramp with an 8mm cutter so you have plenty of tool movement through the cross hole to the solid, then continue drilling.

[MrFish]

Kennametal 4 land drills, B977, B978 etc, will help to stabilize the drill when going into the cross hole, might help .