What's new
What's new

Help me Decide on Standard Tooling! (5-axis Milling)

joeymorgans

Plastic
Joined
Nov 20, 2021
Just got a new Mazak CV5-500 5-axis CNC machine with a 30 ATC. I work in a job shop environment working with mostly aluminium, plastic, mild steel, stainless steel. There is a small chance of doing occasional brass, and superalloys. Components are small to medium sized. I would love to hear your thoughts on how I should decide on my standard tooling.

I want as few tools as possible in order to reduce set up time!

So far I am thinking of splitting up my tooling into the following categories below. I will keep all of these tools set up in holders, either inside the machine or in storage. Then just swap them out when required.

Aluminium / Plastics:
-End mills - standard length - roughing and finishing with same tool - 3 flute - sharp corner - for slotting and HEM.
-End mills - long length rib (reduced neck) - roughing and finishing with same tool - 3 flute - sharp corner - for slotting and HEM.
-Ball nose end mills - roughing and finishing with the same tool - 3 flute.
-Barrell mills - finishing.
-Spiral flute cut taps - M3-M12 - aluminium specific taps.
-Face mills / tipped end mills - 90 degree.

Steels / Stainless Steels:
-End mills - standard length - roughing - 4 flute - 0.5mm radius - for slotting and HEM.
-End mills - standard length - finishing - 6 flute - sharp corner - for better rigidity and higher feed rates.
-Ball nose end mills - roughing and finishing with the same tool.
-Spiral flute cut taps - M3-M12 - specific for steels / stainless (will they break?)
-Face mills - high feed.

General purpose (all materials):
-Thread mills (for doing plate work so you don't have to tap so far into your sacrificial plate).
-Corner rounding tools.
-Carbide TSC drills 5 x D - all sizes required for metric threads M3-M12, and clearance holes.
-Chamfer mills.
-Back side chamfer mills.

Obviously this won't cover everything, but I'm hoping I can do 90% of jobs with only these tools, and just add some special tool where needed.

Let me know if you think anything is missing, if I should split my materials differently, or if you think I should add a bigger range of tools.

Thanks!
Joe
 
Here is what's currently in my machine. Doing similar, aluminum to stainless parts. I use same tap and drills for all materials. If I get a larger qty I will put in material specific, but mostly stick with taps that work well in stainless. This is right next to where I program so it's easy to look and see what is already in the machine. When I take a tool out I attach the magnet next IMG_0858.jpgto the holder.IMG_0856.jpg
 
I like the magnets on the machine! Too bad my tool racks are plastic (Sierra American). If I were to make tags, I'd also include the type of holder and gauge length along with the tool info.

Back to the OP's question: no form taps? Spiral flute cut taps in stainless would raise my stress level.
 
I like the magnets on the machine! Too bad my tool racks are plastic (Sierra American). If I were to make tags, I'd also include the type of holder and gauge length along with the tool info.

Back to the OP's question: no form taps? Spiral flute cut taps in stainless would raise my stress level.
If I could show you my tool library in Cam, tool holders are modeled in. New tools go back in same holder and stickout is updated. A must for 5 axis programming.
 
It's going to depend greatly on your typical parts. For plastic, you'll get best results with cutters designed for aluminum, but that have never touched metal.

For my mix, things vary far too much to use standard tooling.
 
gonna be hard to standardize tooling with only a 30 pocket ATC...
i do primarily aluminum and some plastic, barely have enough space with 31 tool atc. no way i could fit in tools for steels :(
 
For chamfering and spotting I use Sandvik chamfer mill CoroMill 316 2 flutes. It shows incredible tool life in all materials from Al to SS. When needed a chamfer mill for production I use 5 flutes M.A.Ford

Also, I would add shoulder mill for Seel/SS keeping 45 degree face mill.
And use 5 flute rough tool instead of 4 flutes. It slower than 4 flutes in slotting but much faster in HEM.
 
Last edited:
gonna be hard to standardize tooling with only a 30 pocket ATC...
i do primarily aluminum and some plastic, barely have enough space with 31 tool atc. no way i could fit in tools for steels :(
You could keep tools for another material assembled with Tool Offset stickers on them in a locker near to machine and swap tools when needed.
 
-End mills - standard length - roughing and finishing with same tool - 3 flute - sharp corner - for slotting and HEM.
-End mills - long length rib (reduced neck) - roughing and finishing with same tool - 3 flute - sharp corner - for slotting and HEM.
-Ball nose end mills - roughing and finishing with the same tool - 3 flute.
It's pretty common to use the same tool to rough and finish in aluminum. We did it for years. It works, sort of.

But when we started grinding our own tools, we realized we could do much better by having separate roughing and finishing tools. It's not just separating the operations to keep the finisher pristine. Geometries are drastically different.

In your situation, you're already trying to maximize the usage of your tool magazine. Would you even entertain the idea of adding yet more tools?
 
Thanks for all your replies everyone, I appreciate your help.

My biggest concern now is what taps to choose. I have two options:

1. Form taps (one type) for all materials, thread mills (one type) for plate work (so I don't go into sacrificial plate too deep) (will require different sized drills).

2. Spiral flute cut taps (one type) for soft materials, thread mills (one type) for hard materials (can use same size drills).

I suppose option 1 has the advantage of being able to tap much deeper holes. But option 2 will give better quality threads.

Will a general purpose thread forming tap give good quality threads in all materials?
 
Will a general purpose thread forming tap give good quality threads in all materials?
No.

Some materials work harden, some require different H-limits depending heat treatment, plating/anodizing, etc.

Get a couple Bilz style tap holders and swap taps in seconds. Use the right tap for the job.
 
My biggest concern now is what taps to choose. I have two options:
Unless your jobs are substantially similar to each other, which seems unlikely in a job shop situation, I don't see you using standardized tooling for threads. You say you have 30 tool stations; I probably have 30 different threadmaking tools, which I use for different threads in different materials and different situations.

I think the best bet is to setup your tooling for a job while the previous job is running, and not worry about keeping to standard tools. If you try to keep to standard tools, almost none of your jobs will be using optimal tooling. If your quantities are very low, that could be ok, but wasted time using suboptimal tooling can really add up with even moderate quantities.
 
I like the magnets on the machine! Too bad my tool racks are plastic (Sierra American). If I were to make tags, I'd also include the type of holder and gauge length along with the tool info.

Back to the OP's question: no form taps? Spiral flute cut taps in stainless would raise my stress level.
I went with the plastic CT40 snap on tool tags and 3D printed a tool tag holder that sits on the door of my machine. Its been quite nice when swapping from steel to aluminum jobs especially when I need to reuse tool holders, all the critical data is there when I'm doing an assembly.
 

Attachments

  • Tool Tag.PNG
    Tool Tag.PNG
    2.4 MB · Views: 25
  • Tool Rack.PNG
    Tool Rack.PNG
    2.5 MB · Views: 24
Are you a production shop? I am a prototype job shop so don't bother with a 'hard' tool library always in my machines. However I do keep a virtual tool library for tools.
 
For years I was doing something similar to the magnets with my tooling. Recently I decided it was necessary to standardize the tools so it was near impossible to have a tool crash on a first run of a part we have done before. Most of my machines are all Heidenhain Millplus so I'm not sure how applicable this method is for other controls.

In my control my tools are not random pocket, but the pockets do not have to correlate with the tool numbers. Not only that, I can have hundreds of tool numbers. So now every single tool combination, even just a slight change in tool projection length gets a unique tool number. This way if I fire up a program I don't even have to check the magazine. If it comes across a tool it needs that has the holder being used somewhere else the tool number will not be any of the pockets and the control will issue an alarm.

I do typically try to keep the holders in the same pockets of the machine just for simplicity. This way if a job requires a holder to be repurposed the tool that will be needed to be put back will be in the same spot and the whole magazine will be easy to put back to how it was the last time a previous part comes up, rather than having to swap everything around. I assume most larger companies have a system like this with a tool crib but I thought I would share anyway as this has lowered my stress with tools significantly. Rather than need magnets or anything to keep track I just open my tool list in my CAM, and open my tool length offset screen and if the tool number is in the offset list, it is what is stated in my CAM, no exceptions. This has saved a bunch of time since I started this. It can be a hassle to take out a new number to just change the length of a tool by 1/8" or something, but the peace of mind knowing I can walk away and leave the machine running for hours on end on the first part after re-setup is worth it.
 








 
Back
Top