Further Adventures with the Sieg KX3 & KX1

[John HaineParticipant @johnhaine32865]

Somewhere on this forum there's a thread where the use of taps for thread milling was discussed with several contributions from John Stevenson, though I can't readily find it. I did contribute myself and John was very helpful. For my M14x1 internal thread I use two cutters (different trials). One was an M8x1 tap, with all the rows of teeth ground away except one and the tip ground square. That worked well but is limited to conventional milling down into the hole, and unless you also grind away all the teeth but one it will only do one pitch. A single point cutter (like my internal threading lathe tool I discussed) can start at the bottom of the hole and spiral out, climb milling all the way which is quieter and gives a better finish. To generate the code I used a little program provided by Chestnut Pens which Richard kindly modified to allow the use of a tap.

[JasonBModerator @jasonb]

was this it ?

[John HaineParticipant @johnhaine32865]

Aha! Thanks Jason, well found.

From one of my earlier posts in that thread:

After some though I decided that the helix angle of the tap isn't really a problem. You have to remember that the tap is significantly smaller than the hole you are threading. Yes, in principle as the tap rotates the helix may cause some rubbing, but both the smaller tap radius and its form relief are quickly taking the cutter surface away from the work, as it were.

Edited By John Haine on 15/05/2023 09:51:56

[JasonBModerator @jasonb]

Well this will be the last adventure on this version of the forum.

A name plate that will be bent and then let into a recess on a cylindrical part to represent cast letters. They are raised and tapered though hard to tell if they are raise dor cut into the metal from the photo

Plate is 50mm x 32mm letters 3.5mm tall and stand 0.4mm out of the background. Apart from the contour cut around the edge all was done with a 60deg engraving cutter with 0.3mm end width, 0.15mm stepover running at 5000rpm and a feed of 200mm/min. I left it running while I went out to do other things as the run time was just short of 4 hours to get through the 83,000 lines of code.

The machining marks that are just visible on the background cannot be felt and will have disappeared by the time I have silver soldere dit into place, cleaned things up and probably bead blastsed for good measuer.

[Ady1Participant @ady1]

How long did that take to do Jason?

[JasonBModerator @jasonb]

There is a big clue in my post

[Ady1Participant @ady1]

aha!

I was just staring at it thinking omg

But 4 hours wasn't so bad, I thought more like 8

Edited By Ady1 on 03/10/2023 19:45:30

[DiogenesParticipant @diogenes]

..wish I'd been paying more attention to CAD 25 years ago..

[Sarah FParticipant @sarahf]

I’ve been out of action for a while now due to back surgery.  The good news was that it was successful and has reduced the pain in my legs immensly, though it has left me with week and wobbly legs.  Though I have been doing a bit in my workshop before surgery I have not undertaken any of my away from home hobbies for a few years.

I have started racing rc cars again and I have been impressed with the leap in design and engineering.  I could have spent a fortune on a new chassis but I wanted to see how I performed before doing that.  One of the trends has been to use shorter and fatter dampers.  I bought some for my current car, a Tamiya TRF419, knowing I should, hopefully, be able to make the required lower damper towers.  After getting to grips with my CAD programme I came up with a design and exported it as a .dxf file so I could use it with the CAM software Cut2D.  Exporting it as a Gcode to use on Mach3 for my Sieg Kx1 CNC mill.  I did a couple of ‘air’ runs, then a cut into pink foam as it had been a long time since I used the mill.

The profile edges are not rough, its the clear protective film on the carbon.

I did a few test runs to establish feeds and speeds and then cut out the two damper towers.  I did the profiling with a 2mm Routfish cutter at 160mm/min, 7,000 rpm which is  the maximum for the machine.  The carbon fibre sheet was 3mm thick, so I set the CAM software to cut 3.2mm, with 10 Tabs per damper tower (1.5mm long, 1mm high)  I did 3 passes at 0.5mm offset from the final profile then 1 final pass cutting to the profile.  The finish was excellent though there was a miniscule amount of delamination on the underside around the drilled holes, a 3mm Routfish cutter was used for drilling.  I did a little test using the 3mm Routfish cutter to drill a couple of holes and also using a 2mm Routfish cutter to cut a profile inside a 3mm profile.  The 3mm Routfish gave a great finish going in, but a touch of desalination on the reverse.  The 2mm cutter gave a good finish going in, just a minor bur on the outside edge of the hole.  The underside finish was better than the 3mm cutter.

The 3mm test holes, topside.The 3mm test holes, underside

I would be grateful for any comments as to:

Are my feeds and speeds in the right ball park?

Am I taking too many passes, 3 passes for 3mm carbon?

Is it worthwhile cutting to an offset, then doing a finishing pass.

Is there a way to reduce the delamination around drilled holes?  The delamination isn’t bad, it doesn’t stop me using the finished item but it would be nice to have a perfect hole finish.

Any other comments to aid in my work would be appreciated.

(I did use a face mask and had a vacuum cleaning running to suck up the dust)

 

Many thanks,

Sarah 😊

[JasonBModerator @jasonb]

Good to see you are back at it.

 

I can’t help much as I have not machined and CF but would have thought the holes are best done with the 2mm cutter boring it’s way down in a helical path and then moving outwards taking off say 0.1mm as it works it’s way out to final diameter if your Cut2D can do that.

[Julie AnnParticipant @julieann]

The feedrate seems a little slow, about 0.02mm per rev, so the cutter may be rubbing more than cutting. While composites are more abrasive than homogeneous plastic the general rule for plastics is not too fast on rpm combined with high feedrates. The problem with high rpm is that it can lead to the material melting.

On passes I would definitely try doing two steps down and would stick with a final full depth pass to clean up. It looks like a bigger cutter could be used for the profiling, leading to fewer passes, higher feedrate, and less machining time.

For holes it might be better to drill rather than mill. Using drills specifically for composites should eliminate the delamination at entry:

https://www.drill-service.co.uk/products/drills/spotting-and-sheet-metal-drills/dcomp-carbide-drill-sickle-point-for-composites/

Julie

[Sarah FParticipant @sarahf]

Thanks Jason,

I’ll look into whether it will do a helical cut, I can do a 2mm drill and then a second routine to profile out to 3mm dia.

 

I’m running Cut2D v8.5 on an old XP machine.  I’ve also got a Windows 11 machine which I could get a more up to date version if Cur2D.

[Sarah FParticipant @sarahf]

Hi Julie,

Thank you for your reply.  How much of a higher feed rate would you suggest for a 2mm, and a 3mm, Routfish cutter?  The Kx1 CNC mill can only manage 7,000 rpm.

I will try and do the shock towers in two passes, with a final finishing pass.  I set up the profiles with ten tabs, would that seem appropriate?

I’ll get the drill but you suggested to try.  I do have quite a few bits to cut out of carbon so I’m happy with a bit of experimentation.

 

Thanks,

Sarah

[Julie AnnParticipant @julieann]

I would do some experiments starting a 2mm cutter at 200mm/min and 3mm cutter at 240mm/min. The cutters aren’t super expensive so it’s not a disaster if one breaks. I don’t like breaking cutters, but it is all part of the learning curve and pushing limits.

I think ten tabs sounds about right, where they are placed is as important as quantity, usually at extremities and thin sections that are liable to lift under cutting forces.

Julie

 

[EmgeeParticipant @emgee]

Hi Sarah

Just asked a friend who does a lot of carbon fibre sheet machining and copy of his reply below.

These are the right cutters. Use the 2mm or larger.
ROUTFISHM – Carbide Spiral Flute Router, Fishtail point Metric Small

I cannot help you with feeds and speeds as 8K RPM is very low, I would normally feed at around 800mm min with 16000 RPM and do a pass at 1.5mm then full depth.
The carbon sheet has to be fully cured.

Hope this helps.

Emgee

[Sarah FParticipant @sarahf]

Hi Julie,

Thank you for your reply, I will up the feed rate to your suggestion and see how I get on.  Regarding the Tabs I have been leaving it to Cut2D to position them, I will pay more attention to their positioning next time 🙂

Thanks again,

Sarah

[Sarah FParticipant @sarahf]

Hi Emgee,

Thank you for going to the trouble of asking your friend, it was very kind of you.

A feed rate of 800mm/minutes is ballistic!  I am going to try doing two passes, rather and three, and progressively increasing the feed rate.  160mm/minute doesn’t seem too slow when I’m watching, I will just try and imagine it going five times faster 😁

Thanks again,

Sarah

[JasonBModerator @jasonb]

Sarah, I often run at 500-600mm/min feed with my 5000rpm spindle

Remember your 7000rpm top speed would equate to 350mm per min to give the same chip load as the suggested 16000 & 800.

[Sarah FParticipant @sarahf]

Hi Jason,

That’s very interesting, I must read up about feeds, speeds and chip loading.  I have some more bits to cut out of a 3mm carbon fibre sheet, so I’ll do a couple of test runs increasing feed rate each time.  I’ll let you know how I get on.

Many thanks,

Sarah

[JasonBModerator @jasonb]

There are copies of a couple of articles I did for ME in the Worshop section of the website that cover speeds/feeds, have a look at getting the most parts 1 & 2.

As I mentioned I have not been posting much in this thread recently but rather putting parts done on the CNC in with the build threads. I’ve just started a new engine that will have quite a bit done on the CNC which you might want to keep an eye on.

[Author]

Posts