What's new
What's new

Need Help in Maximising Tungsten-Carbide Tool life when Machining Graphite.

bdzhy97

Plastic
Joined
Jan 21, 2019
Hello All :),

First, just a disclaimer: I am a beginner when it comes to CNC machining, only having three months of experience in tinkering AutoDesk Fusion 360 and only one month in Operating an old Taiwanese CNC Machine that uses an old Syntec Controller.

Secondly, I am tasked to machine a cylindrical graphite Stock using a Tungsten-Carbide flat endmill (dimensions are given below) to be used as a tool electrode for an EDM Machine to remove holes from a stainless steel plate for a coffee dripper. So far, things have been a mixed bag for me. I was able to machine one part correctly. The part I am machining is attached below, with the depth set at 5.5 mm.

At the first successful attempt,I tried going for three stepdown passes with the first and second being 2 mm and the last only being 1.5 mm. However, this takes a long time to do (cycle time is upwards of 30-40 minutes for every stepdown pass.) and the code is insanely long, with the whole .nc file itself being 21 MB big. I have decided that to increase the time, I can just use a longer stepdown length of 3 mm and to minimise the risk of the part breaking, I can manually override the Feed Motion to slow it down. Unfortunately, because of my lack of experience, this ended badly with the pins breaking in the part. :willy_nilly: Right now, I am using my previous successful method to machine the graphite even though it takes ages to do.

Does anyone know how I can improve upon my current method of machining this particular graphite stock and is my current method feasible in maximising the tungsten-carbide's tool life?

Thank you,

DeaSk1997

P.S: Here is the link to all the Image and Data of the stock and my Fusion 360 Data: CNC Files - Album on Imgur

Edit: Corrected redundant capitalization of some words as per Milland's request.
 
Last edited:
Why are you running an adaptive toolpath on something like that? I’m not familiar enough with F360s interface to know where to find the stepover on mobile but I would just run a regular pocketing routine with a contour to finish the individual posts if it was critical. If you’re having breakage issues decrease the step down and go to finished size at a slightly slower speed.
 
Hi, here's a few thoughts:

1) Try to use a larger cutter, if you have room for it. A 3mm, or at least 2.5mm. I'd also go to a four flute instead of two, but make sure it's still good for center cutting. DLC (diamond-like coating) if you can get them might help.

2) Better still, get a actual PCD (compacted diamond) edged cutter like this:

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=1213M
Yes, it's just two flute, but the cutter will last forever and give more consistent results.

3) Try spiraling down (helix) to actual size, this will minimize sideward stress on the remnant posts, which is what breaks them. A final pass at the bottom cleans the surface and makes the full length. If you have to stay with regular carbide, monitor edge wear and come to a cut time limit where you replace the cutter before it becomes too dull.

Just a note on readability of your posts. Minimize capitalization of words other than "proper names", unless it's the first word of the sentence. It will help most English readers with following your sentences and understanding your points more easily.
 
Why are you running an adaptive toolpath on something like that? I’m not familiar enough with F360s interface to know where to find the stepover on mobile but I would just run a regular pocketing routine with a contour to finish the individual posts if it was critical. If you’re having breakage issues decrease the step down and go to finished size at a slightly slower speed.

Hi Hazzert,

F360 doesn't have the option to do a pocketing routine and contour for a 2D surface that I have drawn here. Oddly enough, this drawing began as a 3D model of the whole electrode itself. When it was in 3D, I tried to use the regular pocketing routine and used the contour process to finish the individual posts. However, the two processes take longer than the adaptive clearing I did here, and that's why I chose this process. Nevertheless, I will try and revert to the 3D model and machining process and see if I can tinker the feeds and speeds setting of each of the processes to see If I can speed up the process.

Regarding maximising tool life, I have read from a couple of posters here that even though Tungsten-Carbide is still good for machining graphite compared to other materials such as HSS, it is still not good enough to be used repeatedly, and I should pay attention to the feeds and speeds if I want to maximise this Endmill's life. So far, after machining four electrodes, the tool is looking just fine.

If I have any doubts about doing these, I will make sure to post a reply/update regarding my issue.

Thanks!
 
Hi, here's a few thoughts:

1) Try to use a larger cutter, if you have room for it. A 3mm, or at least 2.5mm. I'd also go to a four flute instead of two, but make sure it's still good for center cutting. DLC (diamond-like coating) if you can get them might help.

2) Better still, get a actual PCD (compacted diamond) edged cutter like this:

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=1213M
Yes, it's just two flute, but the cutter will last forever and give more consistent results.

3) Try spiraling down (helix) to actual size, this will minimize sideward stress on the remnant posts, which is what breaks them. A final pass at the bottom cleans the surface and makes the full length. If you have to stay with regular carbide, monitor edge wear and come to a cut time limit where you replace the cutter before it becomes too dull.

Just a note on readability of your posts. Minimize capitalization of words other than "proper names", unless it's the first word of the sentence. It will help most English readers with following your sentences and understanding your points more easily.

Hi, Milland

In regards to a larger cutter, I have tried using a 3 mm cutter instead of a 2 mm one for this Adaptive clearing process, and according to the simulations on F360, it will produce collisions with the stock. However, this might change as I am going to try and use a different method to machine this electrode as per Hazzert's suggestions. I currently have one HSS Endmill that has 3 mm cutter diameter with a 6 mm shank diameter, but I don't think this tool is ideal for repeated machining of graphite, which moves us on to the second point...

An actual PCD edged cutter is rarely sold here in Indonesia, especially with the dimensions of the cutter that I need. I forgot to mention this in my original post, but I am using an ER-20M Tool holder with an ER-20 Collect chuck of 4, 6 and 8 mm inner diameter. The tool that you linked in your reply, unfortunately, will not fit in any of the collet chucks that I currently have. However, I will try my best and see if I can look for one, but I bet it will be even more costly as the Indonesian government has posted import restriction of things over 75 USD. This means that I can't even order the tool itself from an online merchant/marketplace, therefore the online purchase of these tools is definitely out of the question.
[Source: Indonesia to lower overseas online shopping limit to $75 - Business - The Jakarta Post ]

Finally, this brings us to the third point, where for the time being, I have to unfortunately stick to the carbide tools until I can find an actual PCD edged cutter. At first, I chose to just spiral down(helix) in doing a pocket clearing process (when the model was in 3D) but it takes slightly more time, but I will still take your advice in regards to this and the rest of your comment since I think my priority now is to preserve my carbide's tool life.

Oh, and regarding the unnecessary capitalisations..sorry this is one of my bad habits when I'm typing. :wrong:

Thanks heaps for the tips!
 
Last edited:
Rather than machine this from solid, why not just make a holder that takes replaceable graphite pins to the the perforating? Simple brass block with a grid of holes then poke graphite pegs in them? making it the way you are just seams like doing it the hard way!
 
Rather than machine this from solid, why not just make a holder that takes replaceable graphite pins to the the perforating? Simple brass block with a grid of holes then poke graphite pegs in them? making it the way you are just seams like doing it the hard way!

It is pretty typical of sinker EDM electrodes to just make them from solid. With how brittle the material is, and how easy it would be to have angular displacement with pressed-in pins, doing it as one piece seems reasonable.
 
I have made many electrodes like that in my time. My advice, get diamond tooling, or diamond like coatings, every endmill manufacture will have them, the material is very abrasive and will kill a carbide endmill in no time. My toolpath strategy would be to step the posts down one slice at a time, finishing the dia as you go, you will never be able to profile the entire post when you get to full depth without breaking. I would run rpm's with as much as you have, tiny stepdown and fast feerate.
 
I have made many electrodes like that in my time. My advice, get diamond tooling, or diamond like coatings, every endmill manufacture will have them, the material is very abrasive and will kill a carbide endmill in no time. My toolpath strategy would be to step the posts down one slice at a time, finishing the dia as you go, you will never be able to profile the entire post when you get to full depth without breaking. I would run rpm's with as much as you have, tiny stepdown and fast feerate.

Hi 5 axis Fidia guy,

As I have said on my earlier reply to Milland, it will be a challenge getting a PCD or an diamond coated/edged tool in Indonesia but I will try to find one. I also know that the material itself is very abrasive (with it ruining one of my HSS endmills in only a couple of uses in machining other graphite electrodes) and its fine dust dangerous to breathe in. I have taken measures such as buying vacuums to pick up the dust as it is being machined and to wear a protective mask when working with the material. In regards to the toolpath strategy, I have step the posts down as fast and as careful as I can (taking in 2 mm every stepdown) but if that still is not enough than I would like to know how much maximum stepdown length that I should put and how fast is the feedrate to do such an operation?

Thank you, and I look forward in hearing your reply.
 
5 axis Fidia guy is correct about cutting "level first" rather than "depth first".

You mentioned 2mm step down and IMO this is way too much considering the size and also the depth to diameter ratio of the detail. You will need to leave a lot of side stock to do a "thin detail machining approach" so if there is a lot of material left in between the posts then adaptive roughing probably is of very little use here. Also, you will not be able to finish the posts individually in this case either...

If your cutters can last the entire program, I would start with .5 mm depth cuts, and as 5 axis Fidia guy mentioned, cut level first with zero part stock. This is called a thin detail machining strategy. Because the detail is so fragile you will not be able to take any more cuts to adjust the size so what you end up with in the end is what is will be. If it is not correct you will have to alter your program and cut a new piece of graphite. However with this method you will be surprised that you can machine extremely delicate details.

Try to find diamond coated cutters for graphite, they really are the only type which works well for cutting graphite. Uncoated carbide is terrible and HSS is worse.

Your graphite looks very coarse and not dense so small details can break easily. If you can buy graphite which is more dense it will help greatly.
 
Try a path like this, cutting each level first. Also, it can help to use a tool with a corner radius which is no larger than your step down amount.
Image 1.jpg
 
To the OP ..
please listen more to the very good advice You got above.

It is not that Your strategy will not work at all .. it will .. to some extent.

But the Right strategy will work 5-50x more productive in terms of work hours and money made per hour, per person, per tool.

You could not care less, or should not care, if the 70$ tool costs you 150$ imported via DHL.
Just pay it, move on.

.. When it saves You around 300$ vs your best other option.
 
Hi all,
I mentioned in #3 the idea of helixing down to size, circular final pass at the bottom. Using a 2.5mm tool (with 2.9mm pin pitch), this seems to me to be the fastest, safest method once you get the depth per rev down. You could even macro it, so just have X-Y position changes and the macro call for each pin.

But it's not getting any traction, so I'm wondering what's wrong with the idea. ??
 
Try a path like this, cutting each level first. Also, it can help to use a tool with a corner radius which is no larger than your step down amount.
View attachment 247580

Hi, Qwan

I forgot to attach the images of my toolpath and the simulation process earlier on, the link to an album posted above or here: CNC Files - Album on Imgur is updated with those following images. From what I see, my 2-D Adaptive clearing process has similarly followed the process you are proposing. However, I will still try and follow your advice to only go for 0.5 mm depth cuts with cutting level first with the zero part stock instead of going from the side. I also forgot to mention that I have applied a 50% Feedrate Override to my Machine. I am sorry for my lack of experience and the late response, and I am trying to follow other people's advice as well. Please bear with me as I continue to post updates on the process, and I wasn't able to post any sort of reply after the last one yesterday due to the mods somehow marking my posts as spam because of me posting an imgur link.

Thank you for your Patience.
 
If your decrease depth try also decreasing optimal load. Then crank up the ipt to max. I find something reducing optimal load vs ipt increases tool life
 
Hi 5 axis Fidia guy,

As I have said on my earlier reply to Milland, it will be a challenge getting a PCD or an diamond coated/edged tool in Indonesia but I will try to find one. I also know that the material itself is very abrasive (with it ruining one of my HSS endmills in only a couple of uses in machining other graphite electrodes) and its fine dust dangerous to breathe in. I have taken measures such as buying vacuums to pick up the dust as it is being machined and to wear a protective mask when working with the material. In regards to the toolpath strategy, I have step the posts down as fast and as careful as I can (taking in 2 mm every stepdown) but if that still is not enough than I would like to know how much maximum stepdown length that I should put and how fast is the feedrate to do such an operation?

Thank you, and I look forward in hearing your reply.

Where in Indonesia? I did some work in Bandung, we were able to get Sandvik and Kennametal easy enough. I believe they have reps in Malaysia,
 
Hi all,
I mentioned in #3 the idea of helixing down to size, circular final pass at the bottom. Using a 2.5mm tool (with 2.9mm pin pitch), this seems to me to be the fastest, safest method once you get the depth per rev down. You could even macro it, so just have X-Y position changes and the macro call for each pin.

But it's not getting any traction, so I'm wondering what's wrong with the idea. ??

Your idea would work just fine, BUT the tool would have to clear out all the material in between the standing posts, if it does not, the minute you try to clear out that inner material you will break a chunk off and take out a few of those standing posts.
 
Where in Indonesia? I did some work in Bandung, we were able to get Sandvik and Kennametal easy enough. I believe they have reps in Malaysia,

Hi Mike,

I am in Bandung as well and if I may ask, where did you find those diamond coated tools and are they as expensive as they say, especially in Bandung? Also, when did you do the job?? Pretty recently or some years ago??
 
For example a standard 2mm diamond tool could be 4x as expensive. But will last 100x longer. There is no comparison. If you cut graphite regularly invest diamond coated tooling.

Leading edge, YG, widia, cvd all good brands.
 
For example a standard 2mm diamond tool could be 4x as expensive. But will last 100x longer. There is no comparison. If you cut graphite regularly invest diamond coated tooling.

Leading edge, YG, widia, cvd all good brands.

Hi, SteveEx30

Thank you for the brand recommendations, I will definitely look into them. The tungsten carbide one I had only lasted about 7 uses before it failed. I still have 5 more to use but I am not planning to waste any more of them, hence with everyone's recommendation... I will purchase the diamond coated one.
 
Last edited:








 
Back
Top