How does one go about machining a pre existing component rather than just a flat sheet of metal?

This is a concept i'm still struggling to get my head around as the majoity of my cnc experience so far has been on a horribly oversimplified educational system.

To give an example: - say I bought a cheap plastic injection moulded wheel from my local DIY store with a round hole in the centre with plenty of plastic around the edge of it. Now lets say I wanted to machine a hex into the centre so I could drive the wheel from a motor/gearbox with a corresponding shape on the output shaft. I've got the wheel and stuck it in the vice of my machine, and I've got gcode for the hex shape. Now how on earth do I tell mach 3 how to machine my hex in the right place so that the centre of the hex is in the centre of the wheel ?

As a second example, immagine i have a machined a simple shape from a thick piece of steel and I then want to drill holes through the piece at 90 degrees. So I remove the part and flip it round so what was the side is now on the top. I've loaded up my new gcode program but again, how do I ensure it starts cutting the holes in the right place ?

This is something I really need to understand as much of the work I want to do will involve machining things on multiple sides and/or machining onto pre made parts.

Someone may have a more sofisticated answer but basically you need to understand the program you want to use. The program will have an expected place to start. It might be spelled out in the program comments or setup instructions. Most programs I write are set to start at x,y,z zero and that point might be in the middle of a hole in the part or a corner or such like.
 Once you know where that point is, and what it's co-ordinates are you can move the machine manually to there and set the DRO displays to those values.
 For my programs I spell it out in the comments at the top. I usually program the start point as 0,0,0 as I said then it's just a mater of placing the cutter there and zeroing the DRO's. If it's a hole or an edge you can use a center or edge finder manually then zero everything and off you go.

The toolpath display may give some sort of indication as well as to what it's going to do but if nothing else you'll need to be able to read the gcode and see what it's trying to do.


Sage

How does one go about machining a pre existing component rather than just a flat sheet of metal?

Just imagine you are working on a 2D plane

To give an example: - say I bought a cheap plastic injection moulded wheel from my local DIY store with a round hole in the centre with plenty of plastic around the edge of it. Now lets say I wanted to machine a hex into the centre so I could drive the wheel from a motor/gearbox with a corresponding shape on the output shaft. I've got the wheel and stuck it in the vice of my machine, and I've got gcode for the hex shape. Now how on earth do I tell mach 3 how to machine my hex in the right place so that the centre of the hex is in the centre of the wheel ?

Well if you put a plastic wheel in a vice you are gonna break it.

It's a lot easier with Cad/Cam, but expensive.

So i have a part with a hole in it that i want to turn into a hex shape.

I draw the hex in cad with the centre of the hex at X0 Y0

I fix the wheel so that i can machine the hex

I then find the centre of the wheel

I then set the machine to X0 Y0

Now the when i machine the hex it is in the centre of the wheel matching the cad drawing

As a second example, immagine i have a machined a simple shape from a thick piece of steel and I then want to drill holes through the piece at 90 degrees. So I remove the part and flip it round so what was the side is now on the top. I've loaded up my new gcode program but again, how do I ensure it starts cutting the holes in the right place ?

This is something I really need to understand as much of the work I want to do will involve machining things on multiple sides and/or machining onto pre made parts.

Well to make things simple you have a square with a hole in the centre it is 150mm square x 25mm thick

See above procedure to make the square

Then on the side the same principle applies you will make another cad file to match what you want to do

You just set the machine DRO's to match the cad drawing positioning

Now there are wizards for making  Gcode in Mach but it is gonna be much harder to make complicated stuff that way but cheap.

With the expense of Cad/Cam comes built in simulation this allows you to fine tune your machining with minimal breakages.

If you had a collision with a stepper based system it is more forgiving so not too much damage, but not the case with a more powerful servo system

Phil

Dom,
 As for centering the plastic gear, you might want to consider this method. Cut a circular recess in a piece of  MDF (or similar)  with the X & Y DRO’s zeroed.  The recess should be approx ½  the thickness of the gear, (or deep enough to get a positive registration). Start out with the diameter undersize and enlarge until the gear is a snug fit. Now clamp the gear in the recess and it will be centered with respect to the gear teeth which should be more accurate than indexing off the center hole.  The center will be at X0, Y0 assuming the DRO’s haven’t been disturbed during the process. For clamping, drill and tap a couple holes in the MDF and use strap clamps. 

As for drilling two holes 90 deg apart, here is one way. Align the vise fixed jaw with the X-axis and clamp a temp stop to fix the X dim in the vise. (If the stock is small enough maybe use the machinist square to align the stock with the side of the vise). Now after touching off a corner and drilling the first hole, just rotate the stock and clamp it (against the stop, or square) and you have retained your reference, i.e., the stop in X and the vise fixed jaw in Y.

HTH
 al

In regard to the above post, it is assumed that the circular recess in the fixture is centered at X0, Y0. The Gcode for cutting the recess would include something like this:

G00 X(radius) Y.000 Z0.000
G01 Z-(depth of cut)
G02 X(radius) Y0.000 I-(radius) J0.000
G00 Z0.
al

Thanks all for the quick replies.

Phil, you have explained things in a way that makes the most sense to me. I cannot read gcode as if it were english thus I prefer to stick to cad/cam where possible rather than writing everything from stratch. For simple 2D stuff i've been experimenting with a program called CAM BAM which I quite like however for more complicated and 3d parts I have occasional access to stuff like mastercam when I'm able to blag a few hours of time on the computer at my mates machine shop.

So am I right in thinking that the point I specify as the origin in my cam package will be equal to x0y0 on the machine (in work coorinates) thus if I generated a hole toolpath and set my origin to be the centre then wherever i zero'd my machine would be where that hole would be drilled ?

How would go you about finding the centre of the wheel? Would you have to put a tool in the chuck that had the same diameter as the hole and then jog down & zero the axes or is there another / better/easier/more accurate way of doing this ?

How would go you about finding the centre of the wheel? Would you have to put a tool in the chuck that had the same diameter as the hole and then jog down & zero the axes or is there another / better/easier/more accurate way of doing this ?

Normally you would use some form of edge finder, position approx centre then move one axis until you find the edge and zero the DRO, jog the opposite way and find that edge and  type  /2 in the DRO and it will give you exactly half of the distance you have just moved. Move that axis to zero then repeat for the other axis, you have then found the centre of the hole

You could also do as Alenz said above and cut a hole in some material so you can drop the wheel in and clamp it, using the circular pocket wizard would let you do that easily.
Hood

Dom you could do nothing better than spending time in your mates machine shop A LOT OF TIME

There are lots of ways to find the centre of a hole DTI, probe, pointer, to putting a taper point in the collet and bringing it down into the hole.

It all depends on the accuracy you require.

As for holding the wheel, if it was fairly strong you could hold it in a chuck clamped to the table.

MDF would not be the best material for making jigs/fixtures a better bet would be PVC plastic in sheet form this is available from RS components & is easy to machine and is waterproof unlike MDF 

Phil

I've been trying to get some work experience there but he's always got so much work on there would be time to show me how to do stuff. Also a lot of the work is repeat jobs where its just a case of loading a file and pressing the green button. However when he's not so busy and has a new job that requires everything to be done from scratch he's going to give me a call so I can go over and watch and see how its done.

In the mean time I have a machine of my own sitting idle so I might as well try to learn as much as I can through forums, videos and experimentation rather than leaving it to rust in the back of the barn.

Go to http://www.myhobbystore.co.uk/browser/149/workshop-practice-series?p=2 and find the little engineers workshop series of books, there you'll find a few about using milling machines and makeing fitures etc (or try your local libary) these books give loads of info on this sort of thing and are just as relevent to CNC as manual machining.
Also as a general rule keep any referance points as simple as possible, so you example of the block with holes on the top and side you would follow the advise of using the fixed vise jaw plus an end stop. Try to make stops round as well, this helps with swarf etc as your only touching on one little point.

Steve
edit - added link to website.