[zipzit]

I'm a new guy here. Just learning more and more about CNC machining.. (right now playing with LinuxCNC and pyCam)

I'm working on a prototype project, a heavily modified skateboard truck base design. Material = aluminum, probably 6061=T6511 (readily available and inexpensive). Note: this is an item for personal use only.. I doubt I'd ever make more than two or three of them. I have a couple of questions related to that part.

Attachment 264842

Its clear to me that with a simple 3 axis CNC vertical mill, I'm not going anywhere with those drilled holes in the model, and in particular the two holes drilled normal to the angled planes. In fact one of those holes requires reaming for accurate ID control. I'm assuming that I should just remove all the drilled holes from the CAD model.

What I'd like to know, is it acceptable to add a "X marks the spot" locator to help me with the manual drilling setup? I was thinking of actually creating the X score lines in the 3D CAD model using a 'cut' diameter just a hair larger than that of my spherical cutter. My thought was that X mark locator would ease up the drilling layout. I think I can use a drill press and angle plate with enough accuracy to make this work. In the model above I've placed the X just below the large drilled hole as concept sketch. Obviously it would actually be drawn right where that large diameter hole is now.

Comments? How would you proceed to make this part? What is best practice when dealing with holes in general and in this case angled holes?

Thanks,
Zip

[awerby]

I suppose you could do that, but since you've got a vertical mill, why not set up your angles on that, instead of a drill press? It would be more accurate to do it all on the same machine, and vertical mills are usually more rigid than drill presses. But sure, putting the "X"s on there in its first position makes sense to mark the hole locations.

[AARONT]

If you're only making 2 or 3, a 3 axis vmc will work fine.

[sTruGGlebUs]

awerby is correct you should probably use the VMC instead of a drill press.

If you are asking the best method to produce this part in the "real world" it would be an ideal part for an HMC (horizontal machining center). If you want to machine the underside it is a 2 clamping job.
If you can leave the underside stock it is a one clamping job.

The best practice for the two angled holes is to figure out where the center of each hole is (at the plane of their respective angled surfaces) relative to the main (B0) work offset.
Then you can use trig along with known machine dimensions (spindle to center of rotation, work offset value of the "main" offset, known system variables that hold XYZ values of the main offset, print dimensions etc) to calculate the distance from the center of B-rotation to the two points at B0.
Now you can use that distance as a hypotenuse to determine XY distance from B-Center of rotation at any given B-rotation
Now you can convert those XY distances into new work offsets for the 2 different holes
(all this can be done for any of the features that need to be cut at some other rotation than the main offset (B0)
-------that sounds like a whole lot but it is 10-15 blocks of code to do everything I just described in a clean and traceable format-------

By trigging all WCSs off of the "Main" WCS on a part, when you make an adjustment to the main offset all other features follow it correctly--for the simplest example if you moved Y by .002" on the main offset you don't have to also move Y the other offsets.

Some people like to use the B-center of rotation on an HMC as their only WCS (as opposed to WCSs related to the part like i just suggested)---thats a programmer preference thing. The main reason I prefer part based WCS is because my program dimensions will match the part print dimensions so it's easier to read/understand what's going on when you read the code.