Start with a piece that is .75" thick. Mill your piece complete leaving 'clamp material' on the back. Then, flip it over and machine off the excess. Done in one setup
Hi, thanks for the reply
I had the same idea, the only thing I thought is that it will become loose as you start to machine the material away, which could cause a defect.
Please let me know if I am misunderstanding you
I would do something similar, except I would probably start with 5/8" thick material, as that would still give over 1/8" to hold onto in the vise for the first op. Then for the second op I would use soft jaws in a vise that were machined to conform to the part shape and clamp on the part almost all the way up. Then just face off the extra material that was held in the vise initially.
I would prefer to do it in one step like Jason suggested. And when you flip over to machine the back side, instead of vice, use clamps to hole the component. You may have to change the position of the clamps during machining.
Thanks for the reply.
I'm not sure I understand you when you refer to 'one step', surely if you have to flip the material over it is more than one?
Although it would be in one step if the part was machined as I described in the second instance in the original question.
Oh, by one step I meant that major work is finished in one setting. Sorry if I was not clear.
And I don't think 1mm would be a great holding in a vice.
The 1mm doesn't refer to the material which would be held in a vice,but the amount of material left at the bottom of the cut, the material can be as wide as is desired to allow for clamp material.
The method which I think may be the best is to machine all central features, then bolt the part down using the countersunk holes, and machine the outer profile.
This means that the part does not need to be moved/flipped
Would you agree?
Thanks for your replies Deepak
I had thought of that but does that mean you're going to remove the part and re-clamp it again? If yes then you need to make sure that part alignment is correct w.r.t. the holes.
My idea was for it to be like this:
1) Machine all features (3 holes, countersinks, 2 pockets, engraving)
2) Bolt part down (Whilst in vice)
3) Remove vice
4) Machine outer profile
This would work?
How many of these are you making?
One or a "bunch"?
Actually I don't think it would matter to me.
I would clamp to a base of aluminum.
Machine the 3 holes (adding tapped holes into the aluminum tooling plate if first or only part).
Bolt down, remove clamps and finish machine the rest of the features.
One (trivial) simple (reusable) tooling plate with 3 holes.
No change in set-up between cuts. (flip over? why would the part ever need to be flipped? start with 3/4" stock? why?)
Is the start a casting or stock plate?
The extruded cut (showing draft) indicates the part is cast. If machined from raw stock, I wonder if this is needed for function?
I'm with JMather - if you're making more than one make a fixture plate with perimeter clamp holes and the 3 mounting holes.
Clamp a piece of 10mm and machine the 3 holes. Install 3 bolts. Machine the remaining features. Done in one fixturing.
The fixture plate will have a groove where you cut through the perimeter of the part but that doesn't matter.
And if the tolerances or surface finish are critical start thicker and face the plate as the first step.
Even for a one-off piece that's still likely easiest. Unless you do it in one step or use a fixture plate the alignment of your holes isn't going to be precise when you re-clamp it to finish the perimeter (i.e. making sure they are along the true X-axis of the mill).