What tool to spotfacing?

Aluminum22 · Nov 9, 2014

Hi Guys,
Another manufacturing question. I think this is elementary. (I am still learning)

I have 5/8" Cold Rolled 1018 steel Round Rod. I have to spotface a 3/4" diameter into the side of the rod, about .18" deep and drill a hole through that of .26" diameter, centered in the spotface. Then another spotface of equal dimensions gets placed on the opposite side of the rod.

Now, considering that I am using a 14" lathe and have it fixtured to do this (cutting tools in the lathe chuck). Sorry no mill!

What are the preferred tool(s) to go about this?
I want the spotface to be flat.
I want to buy the tools off the shelf.
I understand that a center-cutting end mill will not leave a flat face.
Is there a cutter that can do drilling and spotface at the same time? Or would that be a custom cut tool?

I have at least 200 of these to do, so if I have to pay a little more for better-longer lasting tools I am OK with that.

Here is one type of spotfacing tool: Harvey Tool - Carbide Counterbores - Flat Bottom

I'm sure many of you have good suggestions to simplify the operations and speed things up.

Limy Sami · Nov 9, 2014

Look for ''interchangeable pilot counterbores'' in MSC or the like, HSS will do you fine, and the import tools are quite reasonable $$

Drill hole - sit on peg, spotface one side, flip on peg and do 2nd side, easy peasy metal bashing job, don't over think it, just do it

wgnrr1 · Nov 9, 2014

Aluminum22 said:
Now, considering that I am using a 14" lathe and have it fixtured to do this (cutting tools in the lathe chuck). Sorry no mill!

Step 1, Buy a mill, or heavy drill Press. But preferably a mill. You will need it anyway for more jobs. You won't make it long in the machine shop business without it.
Step 2, What Limy said. Interchangeable pilot counterbores. They will do the job excellently.

Josh

gbent · Nov 9, 2014

How are you going to spotface 3/4 diameter into the side of a 5/8 rod? Spotface depths are called out from full diameter when they are not on flat surfaces.

If you just want the spotface to be .18 deep from the top of the rod, you have good directions. If the part is very long, straightness may become an issue. The spotface will cause the material to curl to the spotface side.

Aluminum22 · Nov 9, 2014

No room for a mill yet, next spring...

Sorry for my deficiency in processes...

So your suggestion is to drill the .26 hole first (hopefully I can get away without having to center drill it)

Then swap out the drill for a counterbore with a pilot of "about .26" diameter (do I make the pilot myself? or do you buy them) I assume it should be a sliding fit, no more? Is this what I am looking for? Interchangeable-Pilot Counterbores | MSCDirect.com

My fear is that is a 3 step process (center, drill & spotface) I was hoping there would be something with one step. Is it possible to have a .26" drill bit inserted into the counterbore? That may be a custom drill? the drill bit would only stick out just enough to break through the other side when the spotface is bottomed out.

johnoder · Nov 9, 2014

hopefully I can get away without having to center drill it

Not happening since you are trying to start on the side of a round bar

Limy Sami · Nov 9, 2014

Have you got a drill press?

It is at least a 2 op job, as a general rule, drill point counterbores tend not to work well / reliably.

Yes that's what you're looking for.

You can buy the pilot or turn a page or two and find the pilot listing - but you can easily make one.

Use a screwmachine drill and you might / could possibly ?? get away without spotting / centre drilling.

extropic · Nov 9, 2014

A 3/4 counterbore uses a pilot with a 1/4" shank. You could have someone custom grind some short drill bits with 1/4 shank however, there is only a small setscrew in the counterbore to retain the pilot. The setscrew will not hold up to retaining and driving the drill.

Also, a counterbore will probably have 3, maybe 4, flutes. I'm assuming that your lathe isn't a solid production type so not as rigid one would like. Same assumption for your set up. Spotfacing that 5/8" bar is going to be an interrupted cut so choke up on the counterbore and feed slowly.

Google 'step drills' to start investigating the option of creating the features in one operation. What you want probably isn't off the shelf and will be a custom, but not hard to find specialists who make them for a living. Such as; Step Drills - ICS Cutting Tools

Aluminum22 · Nov 9, 2014

Yea I do have a drill press, but I was not all that sure how well it would cut the spotface (as it is much less rigid than my lathe)

There are two of these spotfaces on the rod, 6 inches apart. My plan was to mount it on the carriage horizontally.
Cut center
Move over 6"
Cut Center
Change to .26" drill
Drill
move over 6"
Drill
Change to Spotface cutter
cut spotface
move over 6"
cut spotface
rotate part 180 deg
cut spotface
move over 6" cut spotface.

I was hoping there was some tool or technique to get by with fewer operations for the initial drilling and spotface.

If I got a end mill that cut a reasonable flat surface I could cut that first, move over 6 inches and get the other one, then change to the .26" drill, drill hole, move back over to the 1st spotface and drill that, then rotate, put endmill back in and spotface both. That would cut down on the time quite a bit. There must be some sort of endmill that can cut a "reasonable" flat face? Maybe take a center cutting endmill to my local tool cutter?

Aluminum22 · Nov 9, 2014

Thanks for the link Extropic. I will call them and ask if they think that would work for my application. May also make a call to my local tool grinder.

johnoder · Nov 9, 2014

Include a split point on the drill portion to assist with getting started

extropic · Nov 9, 2014

Here's another approach, since you have a drill press.

Make a drill jig with 3/4 drill bushing liners and slip renewable (Type SR) drill bushings, 6" apart. This will eliminate the need for spot (center) drilling and place all holes precisely the same distance apart. Drill all 100 parts in first operation.

For the second operation; Remove one SR bushing from the jig. Install a part in the jig, using a pin (drill bit) in the other SR bushing to align. Remove the second SR bushing. Counterbore both locations, one side (using 3/4 liners as bushings). Replace one SR bushing, reposition and align part, remove the SR bushing, counterbore both locations. Repeat 100 times.

At first blush, a .26 SR bushing with a 3/4 OD isn't standard but may be easily available. Google "drill bushings" and communicate with manufacturers. Worst case, buy SR bushings with 3/4 OD and 1/2 ID then Loctite .26 SF ID bushings inside.

Use toggle type clamps (DE-STA-CO) for quick part clamping.

Designing the drill jig will teach you a lot. Making the jig will (probably) eat up all the time you would save by using it on 100 parts. You may well need to buy additional tooling to build the jig (3/4 reamer, tap(s)). If you intend to expand your machining capability, an may need to make more parts in the future, build the jig.

Aluminum22 · Nov 9, 2014

Extropic, that is something clever I hadn't thought of myself.

I have no problem making fixtures and it is most likely I will be doing these in lots of 50-100 pieces every couple of month. The quicker I can get them done the better, even if it means more time developing a fixture to speed up the job.

Here is my take on your approach. I like the idea and its something I could build.

michiganbuck · Nov 10, 2014

An end mill with an end flute going to center can be sharpened at a good sharpening shop to be flat bottom (Spotface) cutting. Perhaps the best way is to spin grind the end at flat then bring up primary clearance up to just wipe out spin land with having one flute to center.. easy job for a good sharpening shop. The split end or two to center is not as good and may not provide a flat spot. A little more clearance is good perhaps 10*. Short end mill is better. Agree the lathe might have a better spindle than a drill press but with a bushing fixture drill press is OK.
Think 4 or 5 flute best. With locations specifications close a bushing jig as you suggested looks great.
Actually with the .260 you don't need to spot to center but still you would not want a nub in the spot so flat to center is still best..

ap machine works · Nov 10, 2014

Make a fixture to fit your tool post that holds 3 (or more parts) and cdrill, drill, spot face using an end mill or piloted counterbore.

The more parts you fit in the tool post fixture the less tool changes you need to make.

oldbikerdude37 · Nov 10, 2014

Farm the job out to a machine shop.

No 120 parts is not worthy of some fuck around lathe gang fixture even though I love to use a 10+HP lathe as a horizontal drill press.

All you need is a good jig , drill press and a piloted counter bore or two.

extropic · Nov 11, 2014

Aluminum22 said:
Extropic, that is something clever I hadn't thought of myself.

I have no problem making fixtures and it is most likely I will be doing these in lots of 50-100 pieces every couple of month. The quicker I can get them done the better, even if it means more time developing a fixture to speed up the job.

Here is my take on your approach. I like the idea and its something I could build.
View attachment 121581

Well, that was quick. Apparently I underestimated your jig design capability. I can't tell from your model but, I would make the part support (bottom of jig) a V rather than a channel. A V will always center the part and a channel will always rattle with part OD variation.

specfab · Nov 11, 2014

The efficiency of spindle-based drilling and c'boring vs. trying to do this on the lathe is almost infinite. The drill jig is what to do, based on available equipment. There has been no discussion of what the actual tolerances are, though, so there is some ambiguity in what is actually required. Assuming that nothing is highly critical, like +/-.003, my process would be to combine the approach of drill jig for drilling through, then set up a support block and locator pin for the drilled hole as Limy Sami suggested, and fly through the parts doing all one side (2 holes), then reset depth and cycle through the parts again. The c'bore work can all be hand-held, I suspect. The part handling on a simple part like this can be performed quite rapidly by the motivated operator. This minimizes changing tools and bushings to almost zero, which is a big time-waster on a job like this.

Yes, there is slightly more physical risk in setting up to do it that way. Weigh that against time savings overall.

Aluminum22 · Nov 11, 2014

Yes the base of the drill fixture has a v-groove for centering. Plan A is to try this fixture in the drill press. I purchased a counterboring tool (3 flute) with interchangeable pilots. The pilot hole is .25". I am going to take a stubby 17/64 (0.265") drill and grind the OD of the shank down to fit in the pilot. If that works it will save even more time.

michiganbuck · Nov 11, 2014

Very nice fixture that could be used on lathe or drill press. Double bushing is good and with that the .260 could be drilled into base to become the pilot to line up opposite side spot when turning the part. Yes drilling through on first side will do almost the same.
Inserts could be made to accommodate other jobs with same fixture.

What tool to spotfacing?

Plastic

Diamond

Hot Rolled

Diamond

Plastic

Diamond

Diamond

Stainless

Plastic

Plastic

Diamond

Stainless

Plastic

Diamond

Aluminum

Titanium

Stainless

Titanium

Plastic

Diamond

Similar threads