Difficulty to do a both side 3 axis milling program

[ACETRENB]

hey guys, i have a generic 3 axis mill CNC, i am using mach3 to run the CNC and mastercam for g code production and i have some dificulty to think how i can flip a part and machine it getting the right zero so it can be a perfect part, an exemple, i want to machine a eletric guitar, so i have to machine the back first to do the eletronic drilling and so, then flip the stock to do the surface and machine the places where eletronics will go too, i have been reading that i need to do a fixture that when i turn the stock will be in the same place, but i have some dificulties to where the origin part will be, because if the part doesnt get in the center of the stock when i flip and use the same zero home it will be out of the place, so my doubt is i have to use the origin of the part in the edge of the stock, the midle of the stock or what, and how the wcs place thing works in mastercam to use the bottom face as the stock face and if i will need to set a new origin when changing stock plane or use the same origin that comes from solidworks part

Similar Threads:

• 3D Milling Z axis to high on + side of concave surface
• Need Help!- Drifting X-axis, making step ladders one side whereas other side is smooth- SOS
• Need Help!- c axis milling program
• Z-axis - mounting rails on spindle side, rather than tower side

[aarggh]

I find the easiest way is to use locating or registration pins, when creating the design and toolpaths. I include a pin at the top and bottom middle co-ordinates, and keep these in the same position so when the first cut is made, the board is clamped down, the pins holes are drilled and pins inserted, then machine the top, flip, re-insert registration pins, and continue machining the bottom. When I am machining a large complex shape with a very small cutter, I sometimes use a pin in each corner of the job to guarantee the faces line up perfectly.

So long as the pins in the design are the exact same relative distance you can't go wrong.

The pins themselves are simply stainless steel dowel pins off Ebay, they're cheap enough that I buy bags of varying lengths and thicknesses to keep on hand for different jobs.

cheers, Ian

[ACETRENB]

so you use the pin to do the fixture ok that part i got it, so where do you set your home position in the drawing, because the way i see, i can use the middle of the stock as a home position so when i am gonna make the part in solidworks the origin must be centered in the piece, or i can use the edges of the stock as home position and when drawing in solidworks i must calculate where the y and x homes will be to use the stock edge as home position and the center of the part and the center of the stock will be aligned

[aarggh]

I generally center vertically and horizontally all my designs so the registration pins stay in the exact same position for each job, so if I'm machining a 600mm x 600mm job for example, the top pin might be at +275mm and the bottom pin at -275mm along one axis.

And when I surfaced my table, I also engraved 0.5mm deep v groves in decreasing rectangles from the outside edge in, 50mm in at a time, with a v groove right down the middle and across in the middle as far as the travel went, helps like you wouldn't believe having cross-hairs, and alignment grids.

cheers, Ian

[Superman]

so you use the pin to do the fixture ok that part i got it, so where do you set your home position in the drawing, because the way i see, i can use the middle of the stock as a home position so when i am gonna make the part in solidworks the origin must be centered in the piece, or i can use the edges of the stock as home position and when drawing in solidworks i must calculate where the y and x homes will be to use the stock edge as home position and the center of the part and the center of the stock will be aligned

I think you have terminology incorrect, hopefully this may give you a better understanding

- Only the machine has a HOME position
- the part has a WORK ORIGIN
- the program has a WORK ORIGIN

The machine home position cannot be shifted, but the work origin can
- usually controlled by calling up a G54-G59
G54 holds the values for a 3D point ( for a 3 axis machine).
G55 could be used for ...say another job
G59 for yet another
- You need to investigate how to better use this machine feature. I'm sure mach3 uses a work origin shift function.
Programming
You set the part origin in the center top of the stock, make the program, post the NC code
Machine set-up
clamp the stock, put the correct values into the G54 ( incremental distance from machine origin to part origin ), set tools, cycle start ( obviously begin cautious in case of bad programmer or operator settings)


The program origin IS the work origin.
In Mastercam ( like in other CAM systems) the NC program is relative to the part, which is in turn, relative to the graphics origin......the values placed in the G54 (work origin in the machine) is what links the CAM origin back to the machine origin.

[ACETRENB]

thanks superman now i get it, in mach3 we have a program tab called offset where you will tell to mach3 where is the x edge of the stock and y edge of the stock (it will zero the axes , then i put the diameter of the tool to get the values correct), so when i set the edges of the stock in the offset menu i will tell the machine to go 300 on X and 300 on Y then zero all the axes again, if i am machining a 600x600 part, so when i flip the stock and keep it clamped in the same spot it will just do fine, so when i am going to machine a guitar the work origin of it must be at the top center of the guitar, and in mach3 i need to use offset tab to "find" the edges of the stock, then jog the tool (i will have to do some calcs to that) to the top center of the stock, so as the work origin and machine home origin will be at the same spot, then when i flip the stock i will not have problems with alignment, tell me if i am wrong

[Superman]

You are on the right track

This "offset" is an origin shift, it is 3D point around which you have created the NC program.
the point you use in later programming ops in Mastercam, must be the "offset" points you use on the machine

It is the part origin ( & "offset" ) that is referenced back to the machine home position

- for your 2nd operation ( the flip side ) should be set to a fixed point that you can reference consistently ie the center of a drilled hole, a tooling ball, an intersection of 3 faces, etc
you do try to use an actual point on the part if possible, ( or a point on the fixture )
so that you can repeat the part again & again, run the same NC code, at any place you chose within the machining area

[wwendorf]

I actually use the mill itself for this purpose.

For example, I am milling a box that is 6" x 2" out of aluminum that is 6.125" x 2.125" and I am gripping the bottom of the block with 0.1" of my vice jaws.

First, I will put in a tool that is a known perfect diameter, like a 3/8" chamfer tool. I will tell the mill to go to X-.1895 y-1 z-.2, then I put a M0 m5 pause in there. Notice that 1/2 of 3/8 is .1875". I do the .1895 on the first setup so that I have a little "rough material" to get rid of.

Now, I will machine the inside and outside outside of the part, except for the bottom .1" that is held by the vise jaws. The exception is the ride side of the block. I will machine that to finish dimensions.

Now, it's time to flip it over. I do an m0 m5, I remove my part, hit start, and then I will tell my 3/8" chamfer tool to go to position X-.1875 y-1 z-.2 with an m0 m5 after it. The machine will pause again, then I insert the flipped over part, and butt it up solid to the chamfer tool, using it as a stop and tighten my vise. At this point, the rest of my program can run and shave off the remaining .1" of material that was in the vise jaws.

Hope this makes sense. It's kind of hard to explain in writing how it would work. I've been doing this for years and I have <.0005" repeatability.

Wade