I need to mill some sharp corner using an 60 degree chamfering endmill, any advices ?

[ovisopa]

Hello guys,

I just started to use my Tormach PCNC 1100, purchased it in january but only now I had time and confidence that I can start milling something with it, in those months I assembled it (ATC, full enclosure) and also started learning Fusion 360 as I never used that software before, on my other CNC router I only use CamBam, it does the job just fine for all the parts I usually mill in policarbonate shets , aluminum and MDF.

The Tormach machine was purchased because I need to also make some steel cutting dies, and on the router with a 24k RPM / 2.2kw spindle is not the proper way to mill steel.

I'm attaching a photo with the model I need to make, also if you guys think it helps you I can share the Fusion 360 model I made with the part. So far I only milled the exterior contours, and now I have to start milling with some very small endmills (1.5mm) and also to make the side walls as in the model, to form a sharp edge at the top, and hollow in the interior. In this model there are only 2 sharp corners that I'm afraid of (because it can / it will probably / brake the tip of the 60 degree chamfering carbide endmill ) but in the past I also had made some cutting dies, 7075 aluminum , with a shape of a star, and there ware more very tight corners, I also did that in steel on the router, but I never want to try again on the router, it took too much time.



And this is what I milled today :



And for reference only, I will attach a few cuting dies I made in the past on the CNC router, some have some sharp inside corners that I had to mill with engraving bits (single flute)

Steel:


Aluminum:




Now I need to make a similar part in Tool Steel (1.2379) .. I modeled the part using Fusion, and the chamfering carbide endmills I have are from Ceratizit (W0741-S), any suggestions regarding the proper endmills to make those thight corners or any other suggestion like feed and speeds are welcome. I asked the seller about the feed and speed and he opened the catalog and looked in the table, but I know the feeds he told me are not ok when I need to mill with the tip of the endmill, not just the side of it, in the corners I need to ramp up and make each corner look like it radius-less. The smaller endmill I have is 1.5mm, made for steel .. I have some other but I don;t know those ware made for steel milling, some from Kyocera 0.8mm diameter. Anyway, any tool suggestion or a good workflow to not brake the tip of the endmill (not quite cheap at +50€ / each - I purchased 2, one 6mm diameter and one 4, which lost it's tip when I milled the other cutting die on my CNC router, but the 6mm one is brand new)

Similar Threads:

• Problem- No sharp corner
• Need Help!- Chamfering into a square corner
• Problem- Sharp corner lettering
• Want to buy an endmill grinder. Advices please!
• How to make a sharp corner on a mill?

[nutzilla]

Get a custom end mill grinder to the angle you need. Probably cheaper than breaking tips.

[IMT]

I would rough the angle with a regular chamfer mill. To finish, an engraving tool is the only thing I can think of that can make the small internal radius. Since you will be cutting only with the tip of the tool (.005" dia or so) speed isn't a concern, 5140rpm with the 1100.
I would feed it at .0003 to .0005 IPT. It will be painfully slow and the cutters won't last long.
MSC has engraving cutters starting around $8.

Good luck

[tbev]

You'll be fine. Rough out as much as possible and give it a shot with the bits you have at the moment. When I'm trying to dial in a chamfer really exactly I start a little high in Z and go down progressively and take a look each time to see how it turned out. This will help out bc it will act as if you were using more stepovers, removing small amounts at a time.
Give Carl at lakeshore carbide a call, he'll get you set up with custom bits and he will probably have what you need in stock anyways, he's very helpful as well.

Sent from my SM-G900V using Tapatalk

[ovisopa]

Now with the new mill and Fusion 360 software I try to do those kind of things differently, when I made brass emboss stamps on my other CNC router, I first cut a straight wall with a flat endmill, than I used a engraving single flute v-bit with the tip cut to 0.8mm, with this I think the feed is quite high, 400mmpm with a DOC of 0.3mm , this pass takes only a few minutes, but the next pass , the finish pass is made with the same type engraving vbit, but with the tip of only 0.2mm, I used a DOC of only 0.1mm and the feed is 120mmpm. This takes alot of time.

Here is after roughing pass with 0.8mm vbit


And here after the finish pass with 0.2mm vbit


But now I want to mill as much as I can with the side of the chamfering bit, and go really really slow only on corners, with Fusion I think it will be easyer to mill only the corners using ramp up or down movement at a very low feed, and keep a higher feed for the parts when it will mill with the side of the camfering bit.



IMT, your feed rate is in Inces per tooth, this is the formula to calculate in Inches per minute IPM=IPT*RPM*#TEETH ? I want to get a number close to what I usually use - milimeters per minute, so your suggestion is to start from 38mmpm. If the formula is not correct please let me know.

About lakeshore carbide, I heard many good things about the end mills from Lakeshore, the only "issue" is that I'm in Romania, quite far away but I will write them an email, I didn't check if they do international orders also.

Thnak you.

[Steve Seebold]

Why not just have the right size end mill ground with the appropriate angle on the end?

[ovisopa]

Why not just have the right size end mill ground with the appropriate angle on the end?

Steve, I'm not sure I understood you correctly, but I have a 60 degree endmill that fits perfectly with the 30 degree angled wall, but my doubts and concerns are about the very small tip braking when milling the radiused corner, there is so much material left for the small 0.1 or 0.2mm tip. So the endmill I think it's ok for the job, did you wanted to tell me that I need some other endmill.. please explain.

Thank you.

PS> I drilled the holes and made the angled wall using a flat endmill, now I want to mill the interior profile with a 1mm endmill, which I don't like the recommended cutting data, in the Ceratizit catalog the maximum DEPTH OF CUT is only 0.04mm .. Using this depth of cut will take about 1 hour and 24 minutes to make that small profile, that is only 14mm long by 2mm wide






UPDATE.

I milled the interior profile to -5mm, using the 1mm endmill at a very small depth of cut, only 0.06mm and 100mmpm feed rate, 5100 rpm.

Now I need to make the toolpaths for the chamfering endmill , to make the sharp part of the cutting die. wish me luck