What's new
What's new

Looking for materials/drill bit guidance for a CNC milling project.

ghawkinsm

Plastic
Joined
Jan 26, 2017
Hello all, first post here.

I'm designing a jig for leatherwork that requires several very accurate holes, around 1.5mm in diameter and around 30mm deep.

I could use plastic or metal for the jig, and I'm looking for opinions on the best type of material/drill bit setup for this job.

The accuracy is absolutely key, so I can't have any drill-bit wandering. Open to suggestions!

Thanks in advance for any help you can offer.
 
Hello all, first post here.

I'm designing a jig for leatherwork that requires several very accurate holes, around 1.5mm in diameter and around 30mm deep.

I could use plastic or metal for the jig, and I'm looking for opinions on the best type of material/drill bit setup for this job.

The accuracy is absolutely key, so I can't have any drill-bit wandering. Open to suggestions!

Thanks in advance for any help you can offer.

The tendency of the drill to walk would be my biggest concern.
(Assuming these are all blind holes)
I would process the hole this way:
1) spot drill for location
2) Peck drill with a screw machine length, 3/64" drill, as deep as it will go.
3) Peck drill with a standard jobbers drill to final depth
4) Drill/ream with the required 1.5mm drill to depth (2/3rd's the rpm of the drill, and 2X the feed)

Beyond that, I'd send the metal jig out for EDM hole popping.

I'm sure there will be a plethora (finally got to use that word, el Jefe :D) of other suggestions.

Doug.
 
Ok lets define "very accurate", I only ask because you mentioned using plastic for the jig. Plastic jig and "very accurate" don't normally go together.

While doug is spot on with his process, I'm thinking that's overkill. If .005 inch is very accurate I'd say carbide drill in one shot. Multiple steps ending with a reamer is the correct way....just trying to get a frame of reference here.
 
what are you going to use machine wise to drill with and hold the part with? Do you have a milling machine? Drill press? Battery powered hand drill? Quality vise with quality jaws or are you holding the material with your spare hand or foot?
 
If plastic would be good enough, then aluminum will be better, at about the same weight and price, with greater longevity. Good machine, good work holding, solid carbide endmill, I'd be at wide open RPM and a feed rate to give you about .0006 feed per tooth, or. 0012 per rev. (For math I used 400 for SFM and. 060 (rounding in my head) for cutter diameter, and came up with over 25K RPM, so I'm assuming you'll have to adjust downward)
 
Thank you for the detail!

The mill that I have access to has a max RPM of 2500... am I going to have more problems at a lower speed?
 
IMO you will not have problems at lower speeds as long as you adjust CPT accordingly. However with that said like TeachMePlease posted at 25000 RPM it was a chip load per tooth of .0006. With only 2500 rpm that chip load should decrease dramatically. If you run it at 2500 rpm with same chip load you could risk drill walking on you or flexing.


Sent from my iPhone using Tapatalk
 
Thank you for the detail!

The mill that I have access to has a max RPM of 2500... am I going to have more problems at a lower speed?

How many of these holes and parts are you planning to get done? Do you have room on the main part to allow for say a 1/4" - 1/2" hole around the center of your most important hole the 1.5mm one? The reason I ask is it might be easier for you to drill/mill a straight larger hole with precision and leave the more difficult smaller 1.5mm hole to somebody with a lathe that is used to drilling precise and longer length holes. In this way they would make you essentially a drill bushing/sleeve out of material that is agreed to and you just plug it in with a fit that suits you in your part with the larger hole that is easier to drill and you have more experience on? They could mail these parts really easily and coordination and description of the part is really easy.
 
Your whole idea of a drill jig raises big questions.

1) What kind of drill jig has to be drill 20x diameter?

2) What kind of drill jig has BLIND holes? I assume they're blind since you mention that the 1.5mm has to be 30mm deep. Maybe I'm mistaken. Otherwise, just make the 1.5mm hole 6mm deep or so, and counterbore/relieve the remaining depth. If this drill jig is more of a rectangular bar with a line of holes, I'd slot every hole across the narrow width of the bar to allow swarf (or whatever you call leather shavings) to escape from part to part without requiring cleaning.

3) Are you using the term drill jig correctly? A drill jig is an object used to guide a drill into the accurate location in order to drill the work piece. Blind holes don't really accomplish that!

What the heck is this thing doing? Then maybe some real advise can be tendered.
 
Your whole idea of a drill jig raises big questions.

1) What kind of drill jig has to be drill 20x diameter?

2) What kind of drill jig has BLIND holes? I assume they're blind since you mention that the 1.5mm has to be 30mm deep. Maybe I'm mistaken. Otherwise, just make the 1.5mm hole 6mm deep or so, and counterbore/relieve the remaining depth. If this drill jig is more of a rectangular bar with a line of holes, I'd slot every hole across the narrow width of the bar to allow swarf (or whatever you call leather shavings) to escape from part to part without requiring cleaning.

3) Are you using the term drill jig correctly? A drill jig is an object used to guide a drill into the accurate location in order to drill the work piece. Blind holes don't really accomplish that!

What the heck is this thing doing? Then maybe some real advise can be tendered.



I am betting it is not a "drill jig" in the sense we commonly think.
A total assumption on my part, but is sounds like it will end up a "leather punch die" that holds 1/16" pins.....
(might be WAY off base on that though....) :willy_nilly:
 
Thank you all for continued suggestions and advise. Sorry I haven't been clear enough. I'm struggling to explain exactly what this is without an image to support.

I work at a leather goods brand, and we're working on a product that includes a custom-sized leather strap. As you can see in the images, the strap (the brown object) fits inside the jig, which is then closed with the lower object. Depending on the requirements of the strap size, the appropriate holes will then be punched as shown.

When the products are approved, we will use die cutting, but this is early-stage development. The reason for the long holes is so that the punch is perfectly aligned. Even slightly skewed holes completely ruin the end product so they have to be perfect. Laser is not an option because we use chrome-tanned leather which can release toxic gasses when in contact with a flame.

Hope this is clearer now. Thanks again!

CNC Jig.jpg
 
How many of these holes and parts are you planning to get done? Do you have room on the main part to allow for say a 1/4" - 1/2" hole around the center of your most important hole the 1.5mm one?

I posted some images of the jig design. I think the answer to your question is no? Not 100% sure. Sounds like a great idea otherwise...

Thanks again.
 
This question now makes sense.

First of all, you have a fundamental issue on your drawing, that's the square corners on the female portion of the die. There is no good way to make that without die sinking it with an edm ($$$). So at minimum you are going to need to figure out a way to make a reasonable size radius in the corners (~.130" would be reasonable). There are a variety of design tricks to doing that, but that's a separate question.

The material and the holes are the question at hand.

For this application, I think you are going to be unhappy with the soft materials. Plastic will rapidly egg out the holes, and I'm afraid that aluminum will gall when the female and male portion of the die go together, and the punch holes will probably egg out as well.

I think I would probably just use plain old 1018 cold rolled steel. It's cheap and easy to come by. If there is precise thickness tolerance on the male portion of the die, I would use Blanchard ground O1 from Mcmaster Carr for that.

I think you are on the right track with the carbide drill, but a high speed drill would probably get the job done for cheaper, albeit much slower.

I would spot drill the holes with a 45 degree spot to -.035" or so (might as well leave a lead in for the punch). Then peck drill the holes with a carbide drill. 2500 RPM should be fine. I would try and feed at 2 inches per minute, and a peck of .020". Flood coolant or lots of cutting oil. This should be pretty conservative (~45 SFM, and .0004 chip load guess). You could be a lot more aggressive, but this should get the job done.
 
Thanks so much for the advice. The thickness on the male portion is not especially critical, provided it fits within the female portion and enables the jig to function as intended. I will go with the steel and the suggested mill settings.

With regards to the corners inside the female portion, what do you think to this strategy?:

1/16" drill in each corner to required depth
1/4" square end mill for material removal
1/8" square end mill to finish

Thanks again.
 
I think you'd be better served adding a dogbone to the corners and then shopping it out to... well... anyone with a CNC mill can make that. Manual can too, of course, but deep skinny drills need consistent feed and accurate pecks, and you need it right on size. That's a half hour of setup and 20 minutes of run time on a low end CNC, and you don't have to worry about it. $100 job as a one-off.


If you're asking this question, it's going to take you a full day on a manual mill, and you're going to break a couple bits and scrap a couple parts on the way there. You sound like your time is worth more than that.
 
Hi Comatose - thanks for your advice.

I have access to CNC mills but unfortunately very little experience. As I said before, with product development we would typically use die cutters, so this is new territory.

I did reach out to a couple of CNC shops originally but the quotes were significantly higher than $100. Before we graduate to die cutting this time, we'll probably have to repeat this process up to 10 times for adjustments and additional designs (hole placement, etc).

We felt that it would be more efficient for us to complete in-house, in case something was slightly off and could be easily altered. Would be frustrating to be back and forth to a machining shop. Especially at the $$$$ we were quoted.
 
Well, the sharp internal corners adds a zero to the price, no question.

Given that you have access to CNC mills, why not just use the mill to drill your prototypes directly? Or put a hollow die cut punch into the mill's toolholder and CNC punch them, if a drill would tear too much?
 








 
Back
Top