Printable View
About dive into thread milling. Wondered if there is a cheapskate way of tooling up for it.
I believe taps can be modified and that indexable lathe inserts can be used also. Would be most grateful for any advice if you are a fellow skinflint that is ahead of me!
Unless you want to hand grind a single point cutter, you're going to have to spend money.
I'm pretty sure I found a site that was selling them for about £40 a cutter, but I can't remember where.
You could also turn a bit suitable hardenable steel the correct pitch (remember thread mills aren't 'threaded' they're a series of rings), shape it, harden it, then grind to sharpen it.
Hi, I recently got into this and have used both a modified M8 bottom tap (all the teeth on 3 of 4 flutes ground off), and more recently a standard internal insert tip threading tool Experiences described over on the ME site at
http://www.model-engineer.co.uk/foru...p?th=84198&p=6
Look for the later postings in the thread for my contribution, though lots of useful info there. There's a poster there called richardandtracy who has posted a useful application on his website to generate the g-code which I used, works very well.
The standard threading tool was from JB Cutting Tools
http://www.jbcuttingtools.com/epages...493/Categories
though it isn't listed on their website - a phone call might be in order. Usually they have the type number printed on the shank so if you're interested I can look it up when I'm back home.
John.
Gentlemen thanks for the advice. If you could find those tool references I would be obliged.
Attachment 24093
Here's a photo of the tool with the number on the shank, hopefully you can get one from JB. If it would help I could post a photo of the modified tap but it's not very interesting, just an M8 tap with all the teeth ground off except one row. To find Richard's website to get the wizard look for Chestnut Pens.
It would be interesting to see the tap. Here is the link :- http://www.chestnutpens.co.uk/misc/downloads.htmlAttachment 24095Quote:
Originally Posted by JohnHaine
John - Thanks for the info. I actually just bought similar from Banggood. (SNR0013M16 Lathe Turning Tool Holder with 10pcs 16IR AG60 Inserts) Suited my budget at £15.31 with ten inserts included. It will serve to cut my teeth on. Will report on the efficacy.
I use many of their lathe tools and inserts and have found them good value for money. Have cut Titanium for instance,(gently) to good effect. I have no connection with them, just sometimes like relatively good cheapo`s for rarely practiced applications .
Confess this is more an interest in "how to do it" than actual immediate need. May need some foam.
I just started with a chunk of bms.
Tap.
Attachment 24096
If using a tap I think you have to mill down from the top. With a single point tool you can climb mill from the bottom of the hole.
Out of curiosity, how do you measure the effective diameter of the boring tool used for thread milling? I assume that you need this parameter for the CAM tool you are using? I have one of those internal threading tools for use on the lathe but until - eventually - I get my CNC mill conversion done, it's all a bit academic for me...
I simply drill a hole in some MDF about the size of the cutter dia. Harden it with CA glue and finish bore it with the tool. Then measure the hole carefully. This gives me my offset.
Should have said to be careful with various tool tip radii. These will of course vary the cutting dia and thus the depth of the form when trying to match an existing thread. Imagine a huge tip radius verses a tiny one. The V form would cut in different places. Start small and creep up on it.
Best if you download and look at the little app that Richard has on the Chestnut Pens website - that defines the dimensions that you need. I measured mine by clamping the tool in a vee block and careful use of a digital height gauge, it was very quick. The app is designed for metric threads so it calculates dimensions from the standard formulas - it would presumably work for UNF, but I don't think it would for imperial 55 degree forms.
One of the benefits of using a TCT threading tool or a tap is that it already includes the flat or radius. I just used the app, chose my fit class, and it worked.
John - My caution above is born of trying to use standard 55 deg trapezoidal tips which do not always, of course, have a compatible tip radius. Tripped me up until the penny dropped, but close approximations can be found if you search. I have tried it on the CA hardened MDF only so far. But reproduced a heavy Whit. thread quite well,
Hi all,
I'm also hoping to have a go at this - I had a play around with writing the G-Code for it earlier in an effort to better understand what's going on, I've got something that might work - I wouldn't mind a bit of a sanity check on my process, though...
For the sake of argument I'm going to be cutting an M4 thread. For the cutting tool I'm going to use an M4 tap ground down to a flat nose / single row of cutting teeth - I'll be using this tool for both the internal and external threads, but when cutting the external thread I'll adjust the radius to cut me a slightly deeper groove for a bit of clearance (...maybe I'm better off doing that on the internal thread..?)
These threads don't need to be ISO compliant, so long as they work together that'll be fine!
Here's the code I came up with for the external thread (probably ought to be a G17 in there..) along with a vid of Linux CNC running it:
%
G90 G21 G40 G49 M6 T1
G0 X0 Y0 Z5
G0 X-5
G1 Z0 F500
G1 X-3.571
G2 X0 Y-3.571 Z-3.5 I3.571 J0 P5 F500
G0 X-5
G0 Z5
G0 X0 Y0
M2
%
(The radius of the arc is 3.571 as that'll bury a 4mm tap 0.429mm (male thread height) into the 4mm stock to be threaded.
https://youtu.be/J9Zee6phy3o
Does all of this look about right, or wishful thinking..? I guess I'll just have to give it a go..!
Wal.
My CAM uses a radius lead-in to the starting point
I suggest that you start with a bigger thread, seems to me that an M4 tap may be quite flimsy by the time you have ground off 2 or 3 of the rows of teeth. Also it won't give you much clearance in an M4 tapping hole. You do of course need to use a tap with the same pitch as the thread you want which is limiting. I was lucky using a modified tap as I wanted an M14 x 1 thread and had an M8 x 1 tap.
As for the code, I suggest you look at Richard's wizard that I linked to in an earlier post as an example for comparison.
Cheers guys.
Yep, going to try feeding in tangentially as opposed to crashing in to the side like that..!
Hi John - yeah, I've had a play with the Chestnut Pens app - very good it is too. I'm having a go from scratch as I'm a noob when it comes to G-Code and fancy getting my pea-brain around it a bit better. Seems to me that the main difference with how Richard's app works is that he uses full circles and increments the Z at each line, where I'm asking the machine (using 'P') to make a set number of circles while the Z moves as it's doing doing that.
Well, I've ground down a cheap M4 tap, gonna stop my procrastinations and give it a go on a bit of brass... I'm reasonably confident it won't work, but ya gotta start somewhere..!
Wal.
Well I hope it goes OK - the worst can happen is you break a cheap tap, at least it won't be stuck in the hole! First time I tried I was amazed how easy it went, and thread fitted first time.
Well, I'm pleased to report that things went alright... I didn't video my mill doing the deed, so to speak, but the results are below - you can see how I modified the tap in the second clip. Turns out I didn't need to feed in tangentially, I'm coming in from above so it makes no real difference... It's a decent fit but was a little tight to begin with - nothing that running the nut over didn't sort, though.
I'm quite chuffed with the results here - but yeah, of course, it's a hack. CZ121 is forgiving and I wouldn't fancy the chances of this going as well on something harder..! Certainly gets me out of a hole for a little project I've got on the go at the moment.
https://youtu.be/b8TnfNiuA9A
Wal.
EDIT - in action:
https://youtu.be/tV-9vug1Ke8
Nice!
Wal Great job.:applouse: who would have though it.