Hello

Hope anyone can help me ..
I built a milling machine for wood.
Now I would like to mill out a part several times next to each other.
I have the control software Mach 4 ..
Is there a way to create serial parts?

As a CAM program I use Inventor HSM

Thank you for your help

Two solutions if you have big sheet of material and cutting or engraving small 2D/2.5D parts.
1 If you learn manual gcode programming.
Create the gcode for the part as a subprogram, then use G91 relative mode programming in Gcode to make an array of parts by calling the subprogram many times.
2. Buy/borrow a CAM software that can do "nesting and optimization" for you.

If you are making complex 3D or 4D or 5D objects with a 5-axis machine,
You just have to repeat running the gcode after changing the material and loading in at the same offset location defined in MACH4.

I just looked it up and it looks like HSM has a nesting utility. That would be the best way to pack the parts on a sheet, especially if they aren't square since the program will optimize the layout to get the most parts per sheet.

I just looked it up and it looks like HSM has a nesting utility. That would be the best way to pack the parts on a sheet, especially if they aren't square since the program will optimize the layout to get the most parts per sheet.

The FREE "HSM-EXPRESS" cannot do nesting. Fusion-360 also can't.
HSM (not free) has a nesting utility.

It may take some time, but you can manually nest your model in Fusion.
I don't know the geometry of your part so I don't know how well this will work, but in Fusion CAM you can make a linear pattern of your entire setup. 
So you have one model with all your toolpath and you can have multiple parts made just by putting that Setup inside a linear pattern.

 

Now I would like to mill out a part several times next to each other.
I have the control software Mach 4 ..
Is there a way to create serial parts?

I have used G52 several times to do this.
Only takes a few minutes to inset the desired grid pattern and run your part program as a sub.
(right or wrong, it has worked well for me  )
Russ

Hi,
most of the solutions discussed so far involve inducing your CAM program to nest the Gcode.

You could also use g52 or g92 or the parameters 'head shift' or 'work shift' in each fixture (g54, g55, g56....etc).

If you wrote a small macro  that g92'd the width of the part each time it was executed and append it to the bottom
of the gcode (for one part) then run the code a second time the same part will be cut but displaced by the width
of the art from it previous location.

Craig

What is Important
1. Make sure that your router has home switches (+ optional limit switches) to have repeatable home reference.
2. Whether you use a CAM software to do nesting or NOT, you need to know enough of Mach4 Gcodes and Mcodes at least to edit out any gcode/mcodes errors.
so download:-
https://www.machsupport.com/wp-content/uploads/2014/05/Mach4%20Mill%20GCode%20Manual.pdf
3. Autodesk HSM & Fusion 360 list "ARTSOFT" (and not Newwfangled Solution or MACH4) as the vendor to select post-prossessor for MACH4.

Hi,
as satisfying as it may be to have your CAM program nest the parts for you consider this....

The attached picture is a diagrammatic representation of 8 parts to be cut from one piece of material
The first part is cut with work coordinate origin 0,0. The second part, using the indentical Gcode but with the
work coordinate displaced by the g92 offset of x=50mm, y=0

The following code would cut 8 such parts:
g54  (set your work coords to g54)
g92 x0 y0 (ensure no g92 offset is applied for the first part)
m98 p1000
g92 x50 y0
m98 p1000
g92 x100 y0
m98 p1000
g92 x150 y0
m98 p1000
g92 x0 y50
m98 p1000
g92 x50 y50
m98 p1000
g92 x100 y50
m98 p1000
g92 x150 y50
m98 p1000
g92 x0 y0 (Reset g92 offsets to zero)
m30  (end of program with 8 indentical parts cut)


o1000
......
......
(your part Gcode)
.......
m99As you can see the part Gcode is turned into a subroutine by encapsulating it with the o1000 line at the beginning
and the m99 return at the end. It would be necessary to strip any m30 or similar end of program code from
the end of the part Gcode.

Craig

Thank you guys,

You are really great. As for me the topic Cnc is quite new, I still have little experience, but is an exciting topic.

I will try both variants, the HSM nesting option and the Gcode variant. Thanks for the great support. 👍

Ps: Photos of my first serial production will follow