Countersinking carbon fibre sheet with my Sieg CNC Mill

[Sarah FParticipant @sarahf]

Hi,

Over the past couple of months I have been happily cutting out parts in 3mm and 4mm thick carbon fibre sheet on my Sieg Kx1 mill (I will note that having used it a lot I wish I had got the larger Kx3, with the larger work surfaces).

Anyway, I have been using 2mm and 3mm Routfish cutters which have given very good results and I have found  reasonable feed and speeds.

The parts I now want to make require a lot of countersinking, I did try HSS countersinks but they got blunt quite quickly.  My choice appears to be carbide cutters, or a form of a coned burr.  The countersunk holes are for M3 countersunk screws, which according to the research I have done require either a 1/4″, or a 5/16″ countersinking bit.  I’m not quite sure which would be the best.

The carbide cutters come in three and six flute cutters, would anyone know whichever would be better for carbon fibre sheet.

Anyone have any experience using a coned burr for countersinking?

Also has anyone any experience of using a countersink bit in carbon sheet and can pass on any experiences?

 

I am guessing that to get the correct depth of countersink would just take trial and error?

 

Many thanks,

Sarah

[Robert Atkinson 2Participant @robertatkinson2]

I would go for a 3 flute cutter. You can get “countersink cages” which are adjustable depth stops that help acheive consistent countersinks using a hand drill. Standard practice on aircraft.
https://skinpins.com/product-category/skinpin-shop/microstop-countersinks/microstop-countersink-cages/

Robert.

 

[JasonBModerator @jasonb]

Can’t comment on the C/F aspect but a few thoughts on countersinking particularly with CNC.

You have two options. The first is to plunge in as you would with traditional manual machines which quite possibly is not the best bet. Though the advantage of plunging is you get a CSk hole with a slight straight section at the top which better accomodates the screw a sthey don’t come to a sharp edge then it is better not to have the CSK just a sa plain 45deg cut. The off the shelf countersink bits for this have a 6.3mm head and usually come on a 5mm shank.

The far hole was done with the correct size CSk for the M5 screw, the one nearer just a larger one that was taken deep enough to set the head just below the surface which results in a larger hole at the surface.

Second option is to use the Chamfer function of CAM and have a 45deg cutter run around the edge of the hole to a prescribed depth. This allows you to use one cutter for several different diameter holes as well as chamfering any edges. For this I would go with a chamfer mill when working metal but there may be a similar thing specifically for C/F. Provided the cutter is not larger than the standard CSK size you can get the stepped hole so in your case a 6mm cutter would work as it is smaller than 6.3

No need for depth stops you can set the height in the program though may need a bit of trial until you get the right depth. Then make a note and use it in future

 

[JasonBModerator @jasonb]

Regarding sizes, this set have the ISO heads for M3 to M10

[John HaineParticipant @johnhaine32865]

Does a countersink have to have a smooth conical face? Maybe cut it as a set of small steps using an endmill? Saves a tool change. Or use a ball nosed cutter.

[John Haine]

On John Haine Said:

Does a countersink have to have a smooth conical face? […]

That’s a very interesting question, John

MichaelG.

[JasonBModerator @jasonb]

Having seen your comments about drilling in the other thread then the 2nd option may well be the bet.

Although a series of steps may save a tool change it will make the run time longer.

The cutting around the CSK also allows for different sizes and will also CSK things like slots if you have those for say a motor mount

[JasonBModerator @jasonb]

This is how F360 handles it. The CSKs are added in CAD to the required depths. Then in F360 it is just a case of clicking the surfaces to select them and the software will take care of the depths for each hole. I split it into two with the feed rate of the external chamfer set higher than that for doing the holes as the actual feed rate at the cutting edge of the tool is higher on small holes. The purple is waste, it plunges down and takes out most as a CSK would then runs around to put on a final cut. For large CSKs I would probably do it in more than one pass.

[noel shelleyParticipant @noelshelley55608]

Hi Sarah, on thought when working with carbon fibre is the dust or swarf ! If it can get into motors it will be abrasive and very likely conductive, the latter applies to anything electrical. Just a thought. Noel.

[JasonB]

On JasonB Said:

This is how F360 handles it. […]

Very slick !

MichaelG.

[Sarah FParticipant @sarahf]

Hi Robert, I looked at those cages and they look very useful.  I’ve got a lot of holes to countersink, so I was hoping to do it all on my CNC Mill.

 

Thanks,

Sarah

[Sarah FParticipant @sarahf]

Hi Jason,  thank you for the advice and pictures.  The inlet countersunk screw looked a lot better than using a larger countersink bit.

I have ordered one of the ‘Drill Mill 6mm Diameter 90° Point 6mm Shank AlTiN Coated Carbide’ and also a carbide countersink.  A little experimenting is in my future 😉

 

Hi John, I did experiment with doing varying circular pockets, to emulate a countersunk hole.  It does take noticeably more time and I had to be careful tightening a screw into it as it seemed to seat to different depths.  Another problem is that I have noticed I am getting tool wear and need to compensate for it.  Making the countersinks this way would need the tool wear to be monitored.

 

I’ll keep you posted 🙂

[Sarah FParticipant @sarahf]

Hi Noel,

Thank you for your concern about working with carbon fibre, I am wearing a mask and also a vacuum cleaner.

 

Sarah

[Sarah FParticipant @sarahf]

Hi Jason,

That looks quite simple on Fusion, I haven’t tried that software yet.

At the moment I’m using Solid Edge and Cut2D, I’ll see how I can set up to use the V Chamfer cutter. I’m guessing quite a lot of trial and error.

Sarah

[Sarah FParticipant @sarahf]

I’ve just had a delivery of a couple of Routfish cutters and the 90 degree cutter.   Time to start experimenting 😃

 

[Sarah FParticipant @sarahf]

Hi,

 

I’ve not been up to getting into my workshop, but I have spent a bit of time exploring my options with Cut2D.

1) From a CAD drawing, for a 6.35mm countersink into a 3mm hole, I could measure a depth of 3.18mm.  I entered this into Cut2D and it gave a good representation of a countersunk hole.

2) Again from a CAD drawing I obtained the diameter of the countersunk hole, where it breached the material depth of 2.5mm, which was 1.55mm.  I did a profile on this diameter and it produced an oversized countersink, trialling different depths, to 2.35mm, gave a similar size countersink to 1)

3) Using the Pocketing function, on the Diameter of the countersink 6.35mm, to the CAD indicated depth gave a countersunk holes similar to 1)

 

When I’m upto getting into the workshop I will try the three methods and see which is the best 🙂

[Neil LickfoldParticipant @neillickfold44316]

If  you are doing alot of holes, then you want a single point PCD countersink tool. A 45 deg single point chamfer tool. Use a vacuum cleaner to draw the dust away as it cuts help with the tool life . At a minimum you can use coated carbide 90 deg spot drill. With some machines and setups, instead of a centre plunge cut, do a circular interpellation of the hole in a downwards spiral and a complete turn at the bottom of the hole. The interpellation has an advantage of using more of the range of the cutting edge too. Best results come from trial and error.

PCD cutters are really a must with the abrasive nature of carbon composites.

There are desic diamond cutters available that some do like for roughing out of parts etc. These have quite large nodules on them. I think that some are not actually diamond but look like trees of hard chrome to me for some of them.

We use single flute ball mill cutters for cutting 3d shapes on a cnc router , R2 is the smallest we could get at a reasonable price.

Neil

[Sarah FParticipant @sarahf]

Hi Neil,

Thanks for your reply, the PCD cutters are a bit expensive.

I think I will trial my solid carbide cutters first,  but doing the cut as you and Jason have suggested is top of my list to try.

I do use a vacuum to pick up the dust, I can see having to go through lots of dust would be quite abrasive.

I’m hoping to get out into my workshop over the weekend 🙂

 

Sarah

[Author]

Posts