What's new
What's new
By:
Advanced search…

High Quantity Limited Resourse Job

D

DBcooper

Aluminum
Joined
Jul 7, 2017
Location
Kaufman
I was given an opportunity to do a job in my home shop, outsourced from the shop i work for, because theyre swamped right now and my boss is kind enough to give me some work here and there, it benefits both of us.

The job is simple, I need to square up 1000 pieces of D2, +/- .001, with a perpendicularity tolerance of .001" on four sides.

now my question is what is the most efficient way to do this without a ton of consumables? removing about .05" of material per side

ive got a CNC mill and one vise. currently I'm using a 2" APMT face mill.

thanks in advance for your input
 
DBcooper said:
now my question is what is the most efficient way to do this without a ton of consumables? removing about .05" of material per side
Click to expand...

How big are the parts?

If you have amenable geometry I would be doing it in two ops. For op 1 put them in Talon Grip jaws, holding onto the bottom 0.080”, face the top, profile the sides. For op 2 just flip it over and face off the bottom.
 
Put them standing up in a grind vise put it in your big vise on its side to square your ends. Use the small vise to get your stock 90 degree to your big vise. Then let it eat
Don


Sent from my iPhone using Tapatalk Pro
 
I would 100% be doing them in two ops at that size. Probably use a 1/2” end mill for the profiling ops, Helical HEV-5 or something similar. If you use Talon jaws don’t use a hammer and use a torque wrench to avoid overtightening.
 
thanks guys, ill get a set of talon jaws ordered and look into some endmills. my concern of the endmills was high cost of each one, rather than fairly low cost of inserts for the facemill. i guess as long as i buy some good endmills and treat them right, it shouldnt be an issue
 
I would probably try to think up some kind of simple taper gauge I could use for in-process checks so I'm not constantly at the surface plate. Like it has to slide between two dowel pins on a flat surface in either orientation, and not slip between another set (GO/NO GO).
 
Mtndew said:
The same way you would do them at work most likely.
Click to expand...

Normally, I would agree with you, but somewhere along the lines I got something backwards, I do conventional machining at work, and CNC at home, so unfortunately that's not much of an option here lol
 
Is the stock already sawed?
When I have to do stuff like this, I have them either saw or order material that is larger so that I have carrier stock and can facemill the top, and mill all 4 sides. Then I can just flip it over and face it to thickness. (edit: I just realized that was mentioned above)
That is the most efficient way and also ensures that everything is square to the top face and parallel.
 
1000 pcs? You should most certainly look at building some fixtures/pallets for these. I hope you are not planning to run them one at a time in a vise!
 
"D B Cooper" ???

Really?

I think I've seen [what should be] your avitar at the post office. :scratchchin:



-------------------

Think Snow Eh!
Ox
 
D2 is abusive on cutting tools, even in the annealed state. Success is going to hinge on diligently changing out tools as needed. It's nothing like annealed A2, which cuts more like carbon steel.

The real cost of this job is the manual labor associated with constantly swapping out endmills and indexing inserts. The cost of tooling should be built into the pricing. If you can't make this job profitable using realistic (i.e. short) tool life numbers, then you may want to pass on it.
 
I think that I would plan to sqr up 3 sides in the mill with a face mill (much cheaper than endmills) then I would likely plan on bringing it into size (the other 3 sides) in the grinder. And you have plenty of volume to justify buying a clean used one owner grinder.


-------------------

Think Snow Eh!
Ox
 
Is stock supplied and cut? Do you have a good / fast band saw available if it isn't? Do you have a surface grinder? How big is your mill?

I use the squaring method mentioned above (5 sides from top, flip and deck) for onesie twosies, but it might not work out so great here. I could see having some real trouble with the sides of the parts having too much taper, any more than 0.0005" per side and your parts are no good. Endmill wear alone may throw these parts out of tolerance pretty quick, If you mill isn't the most rigid (toolroom type or minimill) It might be a real nightmare.

Edit:

Also - are you going to be able to do these parts in a timely manner? At just 15 minutes per part (which optimistic when you include setup and benching and all the other little things) were talking about 5 weeks (250 hours or so) of work for one person.
 
Last edited:
There are places that specialize in selling squared up stock. That said, maybe you're answering the wrong question.

I never square up stock before making parts on a CNC, it's a complete waste of time. Hold the rough-sawn stock in something like Talon Jaws, mill the top and sides complete, then flip into conformal soft jaws and mill the bottom complete. Sideholes may require additional setups or 4 axis. Can you get the job to make the parts complete?
 
Orange Vise said:
D2 is abusive on cutting tools, even in the annealed state. Success is going to hinge on diligently changing out tools as needed. It's nothing like annealed A2, which cuts more like carbon steel.

The real cost of this job is the manual labor associated with constantly swapping out endmills and indexing inserts. The cost of tooling should be built into the pricing. If you can't make this job profitable using realistic (i.e. short) tool life numbers, then you may want to pass on it.
Click to expand...

i definitely appreciate the input there, i am not nearly as familiar with tool steels as i should be. i am open to any advice in terms of quoting jobs like this as well as one-off jobs.
 
mhajicek said:
There are places that specialize in selling squared up stock. That said, maybe you're answering the wrong question.

I never square up stock before making parts on a CNC, it's a complete waste of time. Hold the rough-sawn stock in something like Talon Jaws, mill the top and sides complete, then flip into conformal soft jaws and mill the bottom complete. Sideholes may require additional setups or 4 axis. Can you get the job to make the parts complete?
Click to expand...

yeah thats usually my philosophy as well, this is just the task that i was given. i wouldnt mind doing the entire job, and its something i can look into, unfortunately i think there is an op that will be done on a turning center (its got a weird profile) which i dont have.. not that i couldnt do it in my mill, but its not particularly efficient to do lathe work on a vmc lol
 
You must log in or register to reply here.

Similar threads

R
Creating a decision tree for internal customer so they can decide what work to send me and what work to outsource.
2
Replies
33
Views
1K
Rough-cutter
R
C
Sacramento Job Shop - Looking for Mill Work
Replies
9
Views
807
EmGo
EmGo
M
Thinking about opening a shop!!!
2 3
Replies
55
Views
4K
Doug
D
M
New Shop- Looking for work/customers
Replies
0
Views
674
Miller846
M
H
Distorting Milling Table While Clamping Work to Table
Replies
9
Views
979
Tyrone Shoelaces
T








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top