Lost drill hole size accuracy in drilling operations

[venta7]

Hello everyone,

Some months ago I've been drilling pin holes (6mm) with very tight accuracy.
The pins were just sliding into the holes smoothly.

But on the last job I've lost that tight size tolerance and now the drill holes are way looser than before.
Even with new drill bit (from the same brand).
Now I need to use 6.2mm pin in order to fit nicely in a hole drilled with 6mm twist drill.
It wasn't the case before when I was using 6mm pins for a holes drilled with 6mm drill and the fit was almost perfect.

I've tried drilling with a drill chuck holder and also with a TTS ER collet holder, the result was the same.
Not even close to the tolerances from few weeks ago.

Here is a link to some videos that I've made measuring the run out of the tools.
https://drive.google.com/folderview?...BkV4RzQDa6q3gm
Please let me know if you have any problems viewing the videos.
The scale on the indicator is in mm, 0.01mm

Could you please advice what would be the reason for loosing that accuracy.
What should I do to fix it.

Machine is Tormach PCNC 1100 and we're working mainly with steel and aluminum.

Thanks a lot!

Similar Threads:

• Drilling a hole using both CTS and drilling a hole through external coolant
• Need Help!- Need advice from the pros - centering a hole and drilling hole pattern
• New Machine Build- Drilling my CRS rails for mounting - what size hole?
• Beginner. What size drill bit for snug fit 12mm hole?
• Drilling a perpendicular hole in drill rod material

[popspipes]

drilled holes are not very accurate, I would put in another op and ream to 6mm.

drilled holes depend on how the end is ground, a bit off center and it will drill oversize.

[venta7]

drilled holes are not very accurate, I would put in another op and ream to 6mm.

drilled holes depend on how the end is ground, a bit off center and it will drill oversize.

Thank you for the reply.
I do understand that, it was accurate enough for my purpose and now the holes are way oversized.
I've also tried to drill with 5.7mm and then use 6mm reamer. That didn't produce better result. Still too oversized for 6mm pins.
Can't figure out what is different now unless there is some tool holder run out, as I mention even with 6mm drill only the tolerance was good for my purpose.

[Steve Seebold]

What material are you drilling? What are your feeds and speeds? What is your peck depth? Did you change the brand of drill you are using?

[wmgeorge]

Thank you for the reply.
I do understand that, it was accurate enough for my purpose and now the holes are way oversized.
I've also tried to drill with 5.7mm and then use 6mm reamer. That didn't produce better result. Still too oversized for 6mm pins.
Can't figure out what is different now unless there is some tool holder run out, as I mention even with 6mm drill only the tolerance was good for my purpose.

Well it used to work fine and now you have some runout or something going on. I would put a dial indicator on your chuck and with the drill bit in the chuck. Try to move the the bit with your fingers or something while the dial indicator present. Rotate by hand with the dial indicator on the bit and etc. Has your drill bit got run out or is it the chuck or perhaps the machine has some wear on the axis?

[popspipes]

Thank you for the reply.
I do understand that, it was accurate enough for my purpose and now the holes are way oversized.
I've also tried to drill with 5.7mm and then use 6mm reamer. That didn't produce better result. Still too oversized for 6mm pins.
Can't figure out what is different now unless there is some tool holder run out, as I mention even with 6mm drill only the tolerance was good for my purpose.

Another thing is I always spot drill first, takes a bit more time but keeps drill "wander" to a minumim when starting the hole.

An old mentor showed me a trick to make a drill drill an onsize hole, he just touched the outer edge of the cutting lip with a stone dulling it slightly, this forces the drill to hunt center and makes it drill a tighter hole. I wouldnt have believed it but I was shown and it does work in a pinch.

[Don Clement]

For locating pin holes I first drill then single point bore and then using this floating reamer holder I built using a 3/8" TTS holder ream to size.

Don

[wmgeorge]

Folks he's using a CNC machine, he does not need to spot drill and it all worked fine before.

[popspipes]

Folks he's using a CNC machine, he does not need to spot drill and it all worked fine before.

If the surface is dead flat, and using a web thinned drill, or preferably a screw machine drill no need to spot drill.

[popspipes]

For locating pin holes I first drill then single point bore and then using this floating reamer holder I built using a 3/8" TTS holder ream to size.

Don

I like your floating reamer holder!, may try to make one for myself......
I also like your indicator holder that fits in the spindle with a dovetail assembly at 90 degrees, I have looked on ebay etc but havent found one like yours, very good idea Don

[mactec54]

Folks he's using a CNC machine, he does not need to spot drill and it all worked fine before.

It does not matter what the machine is CNC or a manual Drill Press a Spot drill is always needed unless the Drill bit is designed to be used without a Spot Drill, there are some quality Drills that are ground so a Spot Drill is not needed, I would say he got lucky with his hole sizes before, a drill Bit unless you know how to grind it can make any size hole you want, over size or on size

Using the Drill Chuck that he has is never going to be very accurate, these drills are some of the best there are if he wants a quality drill Wedevag that will drill on size if his spindle and holder runout is very low and he would need to be using a Screw Machine Drill

North Bay Cutting Tools

Or Ebay https://www.ebay.com/itm/3906-25-64-...ss!37179!US!-1

[CL_MotoTech]

"got lucky"

That's my assessment too. I think OP got above average results and is now getting the results we all would have expected.

In a pinch I've milled/bored pockets with an end mill using a helical path then hit them with a drill as sort of a make shift reamer. This generally is only useful for deep holes where an end mill would't be practical or if you don't have a spot drill. It does provide nice results. The added benefit is it greatly reduces the amount of chip evacuation during drilling and the surface finish can be quite nice as a result.

[Don Clement]

BUMP the main point was that for precision holes I don't rely on drilling but use the boring head and single point bore the hole.

Don

[wmgeorge]

If the surface is dead flat, and using a web thinned drill, or preferably a screw machine drill no need to spot drill.

Correct and its only 6mm hole size and he has done it for months without issues! This is a production line thing, not one off. Something has changed.

[Chris D]

I agree with the comments that something changed between when it was working and now. However, the original process, based on the small amount of details provided, is fundamentally wrong. Drilling a hole for a "slip fit" is not the proper process. Twist drills are not even made to an accurate enough diameter to do this consistently.

The videos showing the indicating process really show us nothing. You have run-out, apparently more as you get further away from the spindle. Does the tool holder fit tight in the spindle? Have you put a shaft in the chuck that you know is straight and round and measured that to see if there is run out? Who sharpened the drill, factory or by hand on a bench grinder? It is very strange that a 6mm reamer is also cutting "Still too oversized ".

I believe you are making a lot of assumptions and you are attempting to do precision machining operation yet you have no way to measure what you have with any level of accuracy. Using terms like "Way looser" doesn't mean much in the world of precision machining.

I would suggest you do the following:

Find a straight 6 mm shaft that you can chuck up with your various tool holders. Put an indicator on it like you have in the video and rotate the tool by hand so you can actually measure to a value as opposed to watching the indicator's needle wobble back and forth.

Check to make sure that you can't deflect the tool holder by pushing/pulling on it sideways while you have the indicator on it.

Assuming everything runs true and your spindle and tools holders are not messed up, review your speeds and feeds, have they been changed since it last worked?

You mentioned that you have tried a new drill and the old drill both with bad results. You also stated that drilling undersized and reaming resulted in poor results. Did you check the size of the hole before the reamer performed its operation? The drill could have drilled oversize and you would believe that the reamer is the problem.

Finally, getting back to the proper process.

In order for a drill to cut on size, it cannot wander when starting the hole. Without a spot drill, the probability of the drill wandering is increased substantially. I would recommend spot drilling to help prevent wandering and the ill effects that will cause.

The drill must be sharpened properly, if it is not, it will NOT cut on size or close to size. If the drill measures 6.1mm in diameter, do NOT expect it to drill a 6 mm hole. In all likelihood, a drill will cut bigger than it is. MEASURE THE DIAMETER OF YOUR TOOLS WITH A MICROMETER so you know what you are starting with. Common twist drills are NOT designed for making holes so close to size you can count on them to give you a "slip fit" every time. They are a roughing tool which is why Reamers are used!

Reamers are ground to very tight tolerances and can be purchased for under/over size applications. They are designed to cut: straight, round, and accurately with regard to diameter.

In my very humble opinion (based on a few decades of doing this) you should:

Spot drill
Drill the hole under size by about .3 mm
Ream the hole with a 6.025 reamer

Be sure to use tool holders that run true
Be sure to use proper speeds and feeds for the materials you are cutting
Be sure to use proper lubricant when cutting
Don't expect the wrong tool or wrong process to perform magically all the time, sometimes luck happens though.

Chris D

[Chris D]

One more thing, have you verified that the material you are cutting today is the same as the material you were cutting last time? A lot of alloys look the same but behave very differently when it comes to machining.

Chris D.

[kstrauss]

What is the red layer in the middle of your floating reamer holder?

[venta7]

Red layer in the middle of the holder? Sorry don't understand what do you mean by that.
EDIT: I see now, interesting build.

[venta7]

One more thing, have you verified that the material you are cutting today is the same as the material you were cutting last time? A lot of alloys look the same but behave very differently when it comes to machining.

Chris D.

Hi Chris,
I've tried after that drilling on the same aluminum material that I have perfect holes with the same speeds and feeds but couldn't repeat that result.

[venta7]

What material are you drilling? What are your feeds and speeds? What is your peck depth? Did you change the brand of drill you are using?

The material is S235JR (calibrated steel sheet), Feeds and speeds (for the drilling operation): 760 RPM, surface speed 14.3 m/min, plunge feed rate 20 mm/min, pecking depth 1.5mm.
I've also tried without pecking since the depth of the hole is 6mm. It was no difference though.
Haven't change the brand of the drill bit.