Spot Facing With Slot Drill?

[Dr_GMJNParticipant @dr_gmjn]

All,

Re. my Stuart 10V build – can I use a slot drill to spot face a casting?

I'm thinking align the drilling head, spot face, then drill the clearance hole.

Cheers.

[Dr_GMJNParticipant @dr_gmjn]

[John HaineParticipant @johnhaine32865]

Yes no problem. Or drill the hole first then you can use an ordinary end mill that isn't centre cutting (unless your intention is to provide a flat face for the drill).

[DC31kParticipant @dc31k]

Posted by Dr_GMJN on 08/05/2020 09:42:03:

I'm thinking align the drilling head, spot face, then drill the clearance hole.

As you mention 'drilling head', please be a little wary if carrying out this procedure in a drilling machine if the only depth control you have is your hand on the quill.

In this situation, the flat-bottomed cutting tool can chatter. Any slight flex of the drilling table also does not help. Sensible use of a rigid depth stop and a strut under the table can improve results dramatically. Experiment on a scrap piece of the same material to get a feel for the operation.

[Neil WyattModerator @neilwyatt]

Among my first self-made tools were spot facers for a 10V.

Turn down the end of a suitable silver steel rod, files some teeth and harden.

They can be very crude and still work:

[Anonymous]

In theory it's not ideal, as a slot drill is ground slightly concave. But in practice it's fine. However, I'd use a different sequence of operations, especially if the surface isn't machined:

1. Spot drill, preferably carbide as it's much stiffer than HSS

2. Drill clearance hole

3. Spot face – while a slot drill is centre cutting if you're spotting only the cutting speed at the centre is zero. Best to avoid that by drilling the clearance hole first.

The above is the sequence I used recently on this rear cylinder cover casting:

Andrew

[Dr_GMJNParticipant @dr_gmjn]

Thanks All.

The work will be done on an SX2 Mini Mill with a chuck.

Regarding the head movement – this is something I did ponder. One recommendation for this mill is to fit a gas strut to more effectively balance the head. I have done this already.

However, with a poorly balanced head (ie it wants to move downwards under gravity), I wonder if this is actually a benefit? Isn't a balanced head more likely to chatter due to backlash on the rack and pinion when drilling, or any operation where the head needs to be moved vertically? It's not so relevant to horizontal milling because the gib can be locked.

Is there a good method to stop a tool grabbing when feeding vertically? I guess using the adjustable z-limit block is an option for restricting the very end on the hole, but it doesn't prevent the heart stopping moment when a tool (eg slot drill) momentarily pulls itself into the workpiece.

Am I over thinking this stuff?

Cheers.

[Dr_GMJNParticipant @dr_gmjn]

Posted by Andrew Johnston on 08/05/2020 10:18:08:

In theory it's not ideal, as a slot drill is ground slightly concave. But in practice it's fine. However, I'd use a different sequence of operations, especially if the surface isn't machined:

1. Spot drill, preferably carbide as it's much stiffer than HSS

2. Drill clearance hole

3. Spot face – while a slot drill is centre cutting if you're spotting only the cutting speed at the centre is zero. Best to avoid that by drilling the clearance hole first.

The above is the sequence I used recently on this rear cylinder cover casting:

Andrew

Thanks Andrew, that makes sense.

[Dr_GMJNParticipant @dr_gmjn]

Posted by Neil Wyatt on 08/05/2020 10:17:07:

Among my first self-made tools were spot facers for a 10V.

Turn down the end of a suitable silver steel rod, files some teeth and harden.

They can be very crude and still work:

Thanks – I've seen that method in my Model Engineering book. However, if I can use tooling I've already got for small diameters like these, I might as well?

[John HaineParticipant @johnhaine32865]

Well, all I can say is that it has worked for me using a slot drill though I would normally lock the quill lever feed and use the milling downfeed, and my mill is a bit heavier than an SX2. I've also used a slot drill in the lathe tailstock in an ordinary chuck to drill holes when I've wanted a flat bottomed hole. Try it and see is my motto, though of course you don't want to spoil a casting.

[Anonymous]

Posted by Dr_GMJN on 08/05/2020 10:27:55:

Is there a good method to stop a tool grabbing when feeding vertically?

For spot facing the depth of cut is small so I just set the depth stop on the quill and use that. For deeper counterbores, like those in the ellipses in the casting shown above done with a 7/8" endmill, I lock the quill and use the knee to move the work rather than the tool.

Generally I find that tools only tend to grab in brass and bronze.

Andrew

[SillyOldDufferModerator @sillyoldduffer]

Posted by Dr_GMJN on 08/05/2020 10:27:55:

…

Regarding the head movement – this is something I did ponder. One recommendation for this mill is to fit a gas strut to more effectively balance the head. I have done this already.

However, with a poorly balanced head (ie it wants to move downwards under gravity), I wonder if this is actually a benefit? Isn't a balanced head more likely to chatter due to backlash on the rack and pinion when drilling, or any operation where the head needs to be moved vertically?

…

Am I over thinking this stuff?

Cheers.

Over thinking is a hazard but I prefer it to brute force and ignorance!

I agree with you in suspecting a balanced head may not be as rigid as one with gravity pulling on it. But chaps who've fitted struts don't suddenly complain of poor finish. Maybe the gib locks dominate, and – if left unlocked – a strut absorb vibration just as well as a heavy head, perhaps better. Could be the ill-effects of balancing out the head's weight are cancelled out by the strut's shock absorbing qualities.

Dunno,

Dave

PS. Not bothered fitting my mill with a strut because I need the exercise!

[Dr_GMJNParticipant @dr_gmjn]

Thanks All.

BTW unless I'm mistaken, on the SX2P there is no option to lock the quill feed becasue there isn't a quill feed. The head can only be moved up and down directly by the rack and pinion using the hand wheel, or the fine feed wheel which is effectively the same thing but with an additional worm drive to drive the rack pinion.

The fine feed on mine was pretty hopeless in terms of adjusting any binding out, so I turned the worm wheel teeth down a fraction, and it's now much better, albeit still with about half a turn of free play…

Ultimately though, even with the fine feed (ie handweheel dog clutch engaged) I think it's the enormous amout of backlash in the whole gear train and its bearings and keys that determines the vertical play.

[Dr_GMJNParticipant @dr_gmjn]

So I drilled the sole plate and box bed on the 10V, and tried spot-facing with a slot drill. It didn't work very well. The sequence was:

1) Align bed and plate, clamp down and calculate middle of assembly and co-ordinates of the holes.

2) Centre drill (shallow cut) each hole in turn (using DROs to get the centres).

3) Tapping drill through both components (using DROs to get the centres).

4) Set depth stop, and drill clearance holes in sole plate (using DROs to get the centres).

5) Re-set depth stop, and spot face the holes (using DROs to get the centres).

I set the DROs to the same co-ordiantes for each hole, to an indicated 0.01mm, and had no issue with the drilling or tapping processes being off-centre. The co-ordinates also matched the cast-in detents very well.

As you can see, none of the spot faces are concentric; if anything they are all displaced outwards approximately diagonally from the centre of the casting. The concentricity error would easily have been picked up on the DROs, so I assume it must be tool deflection.

Fortunately, I erred on the side of caution, and despite them just accomodating the point-point diameter of the nuts (had they been right), the spot faces are a bit too small, so I can correct them. I'll try making a spot facing tool as per Neil's suggestion (although I've no idea exactly how to make and harden the tools!).

Thanks!

[Anonymous]

More likely that the slides moved under the influence of the cutter. If the two flutes are not cutting evenly, which they won't do on a casting, the cutter can easily drag the table. Been there, done that.

Andrew

Edited By Andrew Johnston on 15/05/2020 20:43:14

[SillyOldDufferModerator @sillyoldduffer]

When concentricity matters I prefer not to go the rounds on the DRO, instead changing the tool without moving the table. Slightly tedious even with collets, but, provided everything is locked, the centre drill, tap drill, and milling cutter will all be on the same axis.

You have the same inexpensive DROs as me and I keep an eye on mine! As error tends to accumulate when DROs are moved unchecked over several traverses, I decide on a reference point like a corner and periodically check by returning to it that 0,0 hasn't moved. And rather than zigzagging, I find it safer to cut all the holes on a straight line in one go because then the table moves in only one dimension at a time.

When fitting the DRO make sure the track is correctly aligned and firmly fixed. If not spot on it tends to bend and spring as the head moves causing readings to jump or lose step. Give the XY scales a good test by winding the table back and fro to measure a largish rectangular plate repeatedly: if the DRO is misbehaving, failure to get the same reading ±0.02mm at each point will highlight it.

Lastly, I like to double check positions occasionally with a ruler, divider, markings, or reference points on the work piece.

Even with a high-level of distrust the DROs are faster and less error-prone than dials.

Dave

[Dr_GMJNParticipant @dr_gmjn]

Thanks for the feedback guys.

I did lock the axes before machining.

I did a subsequent test on some plain steel, exchanging the drill bits and slot drill, again with the axes locked, and it still gave a non-concentric circle. Perhaps the existing holes are dragging the cutter off centre? I should have tried cutting the spot face first.

[Michael GilliganParticipant @michaelgilligan61133]

Posted by Dr_GMJN on 15/05/2020 22:34:08:

[…]

I did lock the axes before machining.

I did a subsequent test on some plain steel, exchanging the drill bits and slot drill, again with the axes locked, and it still gave a non-concentric circle. Perhaps the existing holes are dragging the cutter off centre? I should have tried cutting the spot face first.

.

If I read that correctly … it’s worrying

Assuming that the job is properly secured and the X & Y axes are locked: that would imply that the head is moving

Perhaps your concern about the column is worth investigating further.

MichaelG.

[HopperParticipant @hopper]

It's very easy to make a simpler type of spot facing tool, similar to a lathe boring bar made to hold a piece of 1/8" 0r 3/16" square HSS.

Turn a piece of mild steel bar to fit in the drilled hole in your job, with a few thou clearance. Then drill and tap a hole in the end for a small grub screw. A small allen-type high tensile grub screw is best.

Then back from the end a suitable distance, cross drill a hole just large enough for the piece of 1/8" square HSS to fit into. Grind the HSS like a lathe tool bit to cut on the edge facing downwards when the shaft is held in the drill/mill. You can even let the HSS stick out both sides and sharpen both edges. Clamp it in position with the grub screw.Be sure to grind plenty of back clearance on the ends so they don't rub on the curve of the spot faced counterbore.

Or you may even have or be able to buy a suitable boring bar and turn or sleeve the end to fit your drilled hole in the job.

Either way, the end of the bar sits in the hole in the job and keeps the cutter running concentric (well close enough for spot facing purposes).

The cross drilling is easily done by making a drill bushing the same diameter as the bar you want to drill, with a hole up the middle same as the drill size you want to use. Then clamp the bar in the drill vice, with the bushing sitting between the jaws above it where you want to drill the hole. Easy peasy.

I've done this a few times and it works well and is less work than making a "proper" spot facing cutter from silver steel and hardening and tempering it etc etc.

[HopperParticipant @hopper]

Or you can buy a piloted counterbore cutter for 5 quid or less, depending on the selected size, like this one **LINK**

Probably cheaper than making your own!

Edited By Hopper on 16/05/2020 04:43:10

[JasonBModerator @jasonb]

Hopper these are 7BA clearance holes so not much chance od getting a grub screw up the end.

My preference would be to take a piece of silver steel, drill with the same clearance drill that was used for the hole then cut off a small length. Over to the vice and file four teeth in the end then cross drill & tap for a grub screw before hardening.

In use just fit it to a bar turned to fit the hole if not a stock size and away you go. For a small hole like this I may use a longer length of par and simply loctite the pilot into the end.

They can also be used to reverse spot face if needed

[Ron LadenParticipant @ronladen17547]

That's a good tip Jason, thanks I will remember that one. When hardened is the hardness of the silver steel similar to that of a standard drill bit.?

Edited By Ron Laden on 16/05/2020 07:45:21

[JasonBModerator @jasonb]

Probably a bit less and certainly can't be run as fast or as hot as HSS

[HopperParticipant @hopper]

Posted by JasonB on 16/05/2020 07:02:47:

Hopper these are 7BA clearance holes so not much chance od getting a grub screw up the end.

Aha. Impossible to tell from the pic with nothing to give scale. Yes bit small for the HSS dodge.

So what diameter is the OD of the spot face? 6mm or so? Seems like a small and flimsy slot drill would flex and wander easily at that size on an uneven cast surface so your pilot cutter would work much better.

[Dr_GMJNParticipant @dr_gmjn]

OK I’ll give Jason’s method a go. Any tips on making the cutting edge – approximate geometry? And also hardening?

Thanks.

[Author]

Posts