[potomac]

I have access to a Tormach at my maker space. I took a 4 hour class that gives me rating to run it. However, apart from machining the a simple aluminum bottle opener, I haven't had any experience running it or creating CAM files.

I need this particular shape because I will be mounting two very small printed circuit boards vertically, flush against the inner walls.

I know that the hard part will be drilling the holes.

I attached a STEP part here. The message board won't let me attach a STEP file. c case 2.stp :: Free File Hosting - File Dropper: File Host for Mp3, Videos, Music, Documents.

And a screenshot of the part below. It is quite small. 30 mm wide x 20.5 mm high x 10 mm deep




And the basic steps I think (?) I will need to take to machine it.

Please let me know what your frank thoughts are and if there's anything I can do to improve the results!

[Steve Seebold]

I would start by milling the block to size and drill the holes before you cut the center out.

Another way would be to machine it to size, drill the holes then cut the center out as a pocket.

[shred]

Those small radius inside corners are going to need a tiny endmill if done from the side (not optimal with an 1100) or rotate the part so you can drive an endmill through the slot like a football through goalposts. You'll want to be careful how you hang onto it to stop it from collapsing in the process. If that inside radius can be larger then machining as you drew it is a bit more achievable, but you still have to hang onto the parts as you cut them out if you do 3 at a time.

[RussMachine]

Are you only making one part?
If so, It would actually be quicker in a manual mill, since there would be no need for programming.
If you're making several, I would look into buying Aluminum U-Channel, and sawing & facing the pieces to length, then drill.

Anyway,
Here's how I would make it (one part):
1. I would square it up, but leave about 1/8" of extra material in 'Z' height for OP #3 below.
2. Stand it up sideways, and drill the 2 holes all the way thru.
3. Mill the slot out of it. (Extra material left in 'Z' is to to grip the bottom of the part in the vise).
4. Flip upside-down, and finish face mill the bottom, to the correct Z height.

If you use one of those clamp-on, vise-jaw stops, this will be a quick and easy sequence of operations.

[tmarks11]

Could you just use a flat strip of aluminum, drill the holes in it, and then bend it in a metal brake?

Less material, less cutting, much cheaper.

[potomac]

Thanks for the replies. I will reply in order of responses. (For some reason this board is set up to show most recent messages at the top of the thread? Is there a way to change this to normal message board order with most recent at bottom of the thread?)

I would start by milling the block to size and drill the holes before you cut the center out.

Another way would be to machine it to size, drill the holes then cut the center out as a pocket.

Thanks! I will try this

Those small radius inside corners are going to need a tiny endmill if done from the side (not optimal with an 1100) or rotate the part so you can drive an endmill through the slot like a football through goalposts. You'll want to be careful how you hang onto it to stop it from collapsing in the process. If that inside radius can be larger then machining as you drew it is a bit more achievable, but you still have to hang onto the parts as you cut them out if you do 3 at a time.

Currently that fillet is 0.5 mm. What would be a good number to increase it to?

Attachment 351054

Are you only making one part?
If so, It would actually be quicker in a manual mill, since there would be no need for programming.

If you're making several, I would look into buying Aluminum U-Channel, and sawing & facing the pieces to length, then drill.

Anyway,
Here's how I would make it (one part):
1. I would square it up, but leave about 1/8" of extra material in 'Z' height for OP #3 below.
2. Stand it up sideways, and drill the 2 holes all the way thru.
3. Mill the slot out of it. (Extra material left in 'Z' is to to grip the bottom of the part in the vise).
4. Flip upside-down, and finish face mill the bottom, to the correct Z height.

If you use one of those clamp-on, vise-jaw stops, this will be a quick and easy sequence of operations.

I plan on making a handful of them right now and then iterating on the design. The U-shape parts are for mounting optical emitters and sensors so they are lined up perfectly (parallel, hit at dead center).

I had forgotten about U-channel stock, but I'm not sure how parallel you can make the inner walls. Are they perfectly square? There may be a higher tolerance with the ready-made U-channel than if I was to use the Tormach. Looking at pictures here: https://www.google.com/search?q=alum...r=1.34#imgrc=_

The vise jaws are a good recommendation. I will try those too

Could you just use a flat strip of aluminum, drill the holes in it, and then bend it in a metal brake?

Less material, less cutting, much cheaper.

This is a good first instinct, but the constraint of my project is that these optics are lined up well. There may be a tolerance associated with bending that I don't want.

[lens42]

.......Currently that fillet is 0.5 mm. What would be a good number to increase it .

......... constraint of my project is that these optics are lined up well.

The fillet should be as large as you can stand, not as small as you can make it.

If you drill completely through before cutting out the center, the holes should line up no matter how out-of-whack the rest of the machining is.


Sent from my iPhone using Tapatalk

[tmarks11]

...the constraint of my project is that these optics are lined up well. There may be a tolerance associated with bending that I don't want.

Yes, no way you can get a perfect 90 degree bend every time.

Encoder sensor?

[Bryan Turner]

potomac,

If these brackets are for mounting sensors, and the sensors are very sensitive, you may find that the aluminum will 'relax' a little too far once it has been cut to shape, especially for such thin sections.

How precisely do they need to line up?
There are at least three factors I can think of which would affect their alignment:
- Parallelism of facing surfaces
The two sides that have been drilled through are naturally aligned through the drill holes, but after cutting away the center pocket those remaining thin webs will bend inward as well as twist along their length. You can mitigate this by running the part 0.01" thicker (including facing all surfaces so they are newly machined), let it rest on a shelf for a few days, then machine it to size.

- Mounting to a surface
I don't see any mounting holes (I assume the drilled holes are for mounting the sensors), what method is used to mount this bracket to the final location? Assuming it is one of the outside flats, these sections are quite thin and will flex when tightening a fastener against the other mounting surface. In particular the surface they get mounted to must be very flat also.

- Mounting the sensors
At least one of the holes on each side for mounting sensors should be drilled oversized to allow some adjustment of the aim, you may also need to allow for shimming. Laser components are often mounted using 3 screws instead of two so they can 'aim' the beam in two dimensions.

--Bryan

[eltejano]

Get it figured out?