Tooling advice deep pocket

[tcncj]

Need some tooling advice

Need to make some series of parts which have some deeper pockets (110mm)
I can finish the inside with a 20mm ballnose. That's not an issue.

But what's the best way to rough it out?
Material: Aluminium

Should I get a 16mm or 20mm round insert cutter? I've never used those before. I already have a carbide shank for a cutter body with thread.
I don't want to semi finish it after roughing it out. So a cutter with big radius has my preference.
A 16mm long length endmill with 4mm radius would work. But these are quite expensive compared to a insert cutter.

 

[doug8cat]

I don't want to sound rude, but why not talk to your tooling guy. He might give you a great starting point, or better yet an immediate solution.

Good luck,
D

 

[wanispissd]

Deep pockets are a good application for plunge roughing. Basically drilling with the endmill, with some overlap of the row of holes.

Obviously, tool needs to be capable of straight z plunge.

Sent from my Pixel 4a using Tapatalk

 

[imachine909]

What is the rough length and width of the pocket?

 

[Hardplates]

I'd drill a hole and then plunge rough it with a long high feed mill. But I don't work with much aluminum so I have a lot of high feed tooling which works very well for plunge roughing since it's designed to cut on the face of the tool and long lengths are common.

 

[imachine909]

Should I get a 16mm or 20mm round insert cutter? I've never used those before. I already have a carbide shank for a cutter body with thread.
I don't want to semi finish it after roughing it out. So a cutter with big radius has my preference.
A 16mm long length endmill with 4mm radius would work. But these are quite expensive compared to a insert cutter.

If the walls that appear to be 90 degrees to the floor truly are then the round inserts will be slow. Being that you can only step down half the diameter on the inserts. That is if your machine can handle the cuts that deep.

You don't want to semi finish? Well at those lengths and any kind of roughing feed rate and DOC you will have deflection and most likely will result in garbage finishes due to unpredictable WOC on finishing.

Sounds like you are on a tight budget so going with any tool that will fit the carbide shank you already own will be the cheapest way to get the parts done.

More information like how many part, max RPM, length and width of pocket, high speed machining options. The answers to question like these will help with the feed back you receive.

 

[tcncj]

What is the rough length and width of the pocket?

Around 300mm x 200mm

I'd drill a hole and then plunge rough it with a long high feed mill. But I don't work with much aluminum so I have a lot of high feed tooling which works very well for plunge roughing since it's designed to cut on the face of the tool and long lengths are common.

High feed tooling doesn't work well in Aluminium

If the walls that appear to be 90 degrees to the floor truly are then the round inserts will be slow. Being that you can only step down half the diameter on the inserts. That is if your machine can handle the cuts that deep.

You don't want to semi finish? Well at those lengths and any kind of roughing feed rate and DOC you will have deflection and most likely will result in garbage finishes due to unpredictable WOC on finishing.

Sounds like you are on a tight budget so going with any tool that will fit the carbide shank you already own will be the cheapest way to get the parts done.

More information like how many part, max RPM, length and width of pocket, high speed machining options. The answers to question like these will help with the feed back you receive.

No tight budget at all. A simple endmill with corner radius will do the job but rather invest in a new tool if that gets the job done faster.
Just curious which the best tool for the job is.
I have never used round insert cutters (tool rep recommends these). But I'm told that these are "old" and they get replaced by high feed cutters.
The walls are angled by the way

 

[OVodov]

I just made part with 5 inch deep pocket from 6061. So I would suggest you for finish the biggest cutter you could find but radius of this tool must be smaller than radius in corners of the part.

 

[OVodov]

For funish better to take solid carbide tool with neck. Length of the neck should be no less than depth of the pocket. Hold this tool in shrink fit holder. Tool in ER will deflect. For roughing use any indexable cutter you have

 

[OVodov]

So in my case it was 5 inch deep 7” long and 6” wide pocket with corner radius 6.5mm. For roughing first I used 2” Face mill that could reach 4.5”. Then 1” indexable cutter to the bottom. Both of them I used with TSC. For finish I used 0.5” end mill. First remachined corners and than finish all walls.

 

[tcncj]

Thanks for the replies.

Toolrep recommended me this:
XP08 Aluminum Router For Maximum Performance | Seco Tools - YouTube
And I think it will save me quite some time when doing some quick simulations.


I have special tools for finishing. That won't be an issue.

 

[OVodov]

Kinda jealous.
Seco is great brand. But I don’t have it.
Using Mutsubishi AXD4000 here.

 

[imachine909]

Here is what we use
Walter Tools milling Skytec M2131 ramping milling cutter: aluminium wrought alloy aircraft industry - YouTube
This tool will run at recommended speeds and feeds with the right machine. Skip ahead to 1:50 on the video for the actual cutting.

The Walter will be much faster than the Seco, if the machine can run at speeds and feeds needed.

 

[Hardplates]

High feed tooling doesn't work well in Aluminium

Actually for plunge roughing and super long reach it works quite well. Not as well as a dedicated aluminum tool but will get the job done in a timely manner.

 

[blackwolf4278]

Need some tooling advice

Need to make some series of parts which have some deeper pockets (110mm)
I can finish the inside with a 20mm ballnose. That's not an issue.

But what's the best way to rough it out?
Material: Aluminium

Should I get a 16mm or 20mm round insert cutter? I've never used those before. I already have a carbide shank for a cutter body with thread.
I don't want to semi finish it after roughing it out. So a cutter with big radius has my preference.
A 16mm long length endmill with 4mm radius would work. But these are quite expensive compared to a insert cutter.

Okay, so I can give you a definite solution for roughing this thing. I'm roughing a 4.5" deep pocket.

What I use:
2" Insert Drill -> I drill 3 holes then I'm left with walls to rough
I go in with a 1.25" DIA High Feed cutter, cutting .050" for Depth of cut, at about 6k RPM and 240 IPM

The pocket I'm cutting is 4.5" Deep, 3.93" Long and 2.8" Wide with R.625 Internal Corners, my cycle time is 11mins.

If you need more details PM me.

 

[Winterfalke]

The 2" insert drill is also what I was going to suggest. Doing similar sized pockets I would open it up with the big 2" drill (stolen from the lathe guys) then rest rough with a 3/4" insert tool. Workholding was always my limiting factor, so whatever rougher you can push and not pull the part out. Through spindle coolant was always a big plus for any sort of pockets, even toolholders with a coolant slot alongside the tool is better than flood for clearing out the chips.