Stress relieving 304 stainless questions

[aluminum2]

I am having a lot of difficulty machining a 2" x 80" diameter piece of stainless steel on a lathe and keeping it flat. I need to machine the part flat within .03" and so far the best attempt was .04" and the worst was about .08". The part is measuring within .008" flatness when clamped in a 4-jaw chuck, but as soon as it is released, it starts looking like a Pringle (exaggerated). I don't know much about stress relieving so I have to have to ask the following questions.

We get the plates heat treated at 1030°C, Does this mean the plates are stress relieve parts starting out or is this a separate process?

Does anyone know of a good resourse that tells you how to stress relieve a part? My company has an oven for curing paint which could be used to stress relieve the part between machining operations.

 

[EdStainless]

How many steps are using in the machining?
The problem with annealing stainless steels (and the alloy does matter a lot) is that differential (non-uniform) cooling will cause residual stresses.
Is this coming from round or plate?
What is the original stock size and finished size?
What other machines do you have available to so this on?

= = = = = = = = = = = = = = = = = = = =
P.E. Metallurgy, consulting work welcomed

 

What is the product form? I will presume round bar.
If the work is done on a lathe then flatness cannot be a criterion - please be more precise in your description.
Your raw material arrived annealed as per customary, so my only guess is that the cooling from 1030°C was not uniform.
The first thing you need to work out is how much of the unstraightness in this slander part is due to gravity.


"Everyone is entitled to their own opinions, but they are not entitled to their own facts."

 

[aluminum2]

How many steps are using in the machining?
- currently 3 processes. Machining the face and OD. Flipping it, then Machining the face and OD. Then flip it back over to the original side and skim cut it.

Is this coming from round or plate?
-From what I understand it is plate that has been flame cut into a round shape

What is the original stock size and finished size?
-Original stock size is 2.25" thick. Then machined down to 2.035". It is either skim cut or .050" depth of cut.

What other machines do you have available to so this on?
- Only have a vertical mill turn that can handle a part of this size. It can be milled or turn flat, but we turn it.

 

[aluminum2]

The supplier certified the material to the asme sa 240 specification, but I do not have the spec to know what that means or if cooling rate is requirement. while machining, the plate is well supported in the center. When it is inspected It is placed on beams so the forklift can get under it. I ran it through FEA for gravity and the computer said that it would effect flatness by.002".

 

[EdStainless]

I presume that the plate is nice and flat to start with. How flat is it?
Since it is only 2.25" to start with I am going to say that if the shape changes it is mostly the result of your machining stresses. Plate cools fairly uniform from anneal (usually in a continuous plate mill).
I would consider milling this. You could take material from one side, turn it over and shim for any non-flatness, finish the second side, then when you turn it back over it should be flat on the bed and you can finish the first side.
I suspect that you are pushing too hard on it. Be careful with a skim cut. Taking a light pass on SS that is work hardened from the previous pass can be a real challenge.

= = = = = = = = = = = = = = = = = = = =
P.E. Metallurgy, consulting work welcomed

 

[aluminum2]

The plate is usually around .08 out of flat. I think these plates were pressed flat, but I don't see that clearly labeled in the cert. While machining they encounter interrupted cuts because they do not want to take more than .050" Depth of cut. Do you think the interrupted cuts are causing sections of work hardened material? The machinists did encounter work hardening with .010" passes and it was a nightmare for them.


I was considering milling this with a 4" 14 inserted cutter. The lead angle is 45 degrees so I am not sure if this will put too much pressure on the part. Any reason why milling would work better over turning?