Ive been working on my airsoft AR upper receiver that will go with the lower ive done and have been doing a lot of research for tooling options, so i figureed Id ask here as well and see if anyone has some input.
Im on a 1100M, plan on milling the Picatinny rail 1st op, then hold the stock in the Micro Arc in a custom fixture on the rail, bore the hole and do all the other milling on the 4th axis, then Op 3 bottom “open” side of part in a 3 axis fixture. The part will be Alum 6061-T6. The bore is 1.035, and I will hit if from both sides to a depth just over 3 7/8. Part/hole length 7.665.
I currently have a quote for a super long reach, necked end mill with chatter-reducing flute geomotry. with AB tools. This tool is 345.00.
Also have a quote for a 1.035 reamer, and this tool is 495.00 bones!
I also looked into Allied technologies for the possibility to drill this hole. The engineer there says it’s doable based on the machine’s power curve but it comes down to shank size using the TTS holders OR even the ER-32 collet holder. The smallest shank they have is 1 inch. Also, many have told me the power of the machine is really a challenge for drilling such a big hole.
I worked with Nick at AB Tools to come up with the tool geometry here are the drawings. His recommendation is to pocket mill at multiple depths till i hit my total depth instead of a standard boring operation, explaining that the tool load will be reduced going with this type of tool path.
Im looking for any input you guys have regarding super long reach milling and reaming, as well as off-the-shelf tooling options that won’t break the bank like these tools are going to.
Has anyone used the modular insert tool heads Tormach sells for anything this deep? IF so, what one did you use?
A decent boring head and boring bars shouldn’t have a problem with 4” depth. Likewise a suitable long end mill, but then TTS gets to be an issue. Maybe look at getting a long 3/4” end mill and installing a TTS collar onto the shank.
Big drills are annoying because they take a lot of torque at slow speed so you have to shift the machine to low belt and hope the tool doesn’t spin in the chuck or collet or get stuck, especially if you’re going to be hanging the part off the end of a Microarc..
I wouldn’t bore it attached to the MicroArc. It’s not strong enough to hold position on entry. Bolt to the table and drill/bore the part. Then leave the tool in the part to use for alignment as you bolt it to the MicroArc. Or attach to the MicroArc and clamp the bottom in a vice. The MicroArc holds pretty well but I always steady my parts on the Y axis, because the MicroArc will move a couple tenths of a degree.
How big is this hole?
I’m not an expert on this but I would think you could cut the pocket (aluminum is easy to circular bore mill with a long aluminum end mill) in one shot and then just ream it to size?
They also have long reach square end mills that can work. High feed style end mills have worked well for me on long reach operations, and the chips are easy to evacuate with air/mister coolant.
This is a great idea. Are you talking about this press fit type collar from Tormach, Or a standard shaft collar? And would it need to be anything specialized for balance or just a run-of-the-mill shaft collar from McMaster?
One idea I have been thinking about to mitigate this issue on the Micro Arc is, I was thinking of making up a precision fitted support block I would slip under the stock for the boring or drilling operation while milling and reaming the bore. It would transfer the load directly into the table. ? I feel like this would work quite well, what do you think?
Hole is 1.035.
That’s the current plan, mill to 1/2 way then bore to 1/2 way.
This is perfect and just the right kind of cutting geometry to reduce chatter. But they have another tool with a longer necked reach, less tool holder end shank, which is better because I can get a bit deeper. Thank you for the recommendation and the time to look it up, much appreciated!! and its off the shelf!
Question now, is the downside to this tool that it is only 2 fluter? Im going to look to see if they have 3 Fl.
The 2 flute design on the high feed cutter is needed to help clear out chips because of how gummy and sticky aluminum can be. I would stick with the two flute because of how this cutter geometry works. High feed milling is not a quick strategy for material removal but its is great when you are pushing long reach or very deep slotting.
You could also get by with one of their necked 3 flute end mills which are in the same band of 150-180 USD. Good luck to you on the job!
Thanks John. I called Helical today after I saw your post and the sales rep is telling me that this tool geometry could work, but not necessarily the best option for super deep pocket milling.
Have you used this tool for really deep milling?
I am seeing other 3 flute tools that could work as well.
I would definitely like to hear what the rep had to say.
My reasoning for HFM use is that Tormachs are maybe not well suited for large diameter tooling sticking really far out. This creates a large torque arm when you use traditional side milling techniques. By using HFM tooling that radial force is now axial and pushing upwards into the spindle. This was my approach to expand the capacity of the machine with the TTS er16 collet system that I was using on a 1100PCNC. Additionally the chips the cutter makes are small triangular “C” shaped and are easy to manage with a mister and can be easily blown out of a slot/bore. Its slower than traditional strategies but in deep profiles its been stable and reliable for me.
On an 1100 PCNC I ran Helical #84457 at 4800 RPM and 110IPM and 0.015”/0.020” axial pass with a 2.000” reach.
Yeah, they are so you can keep tool length offsets with the TTS ring indexing on the spindle geometry.
I’ve shrink-fitted them and/or glued them on with #620 loctite and they held up fine, but if you’re just doing a one-off or proof of concept, you can just get a 3/4” shank or R8 tool and set the tool length when you put it in the machine.
