[davejpc]

I have just finished converted my VTM machine to CNC and now ready to produce my first machined part.
As a starting point I have written the GCODE to make a crankshaft for the 5" PANSY loco. It seems to work ok when tried on a trial piece of wood, with the depth set very small just to get an idea of the outline and all seems good.
What I don't understand is how I would progressively mill to the final size the mild steel. When I manually do this I would take a small cut off all around the profile, repeating this gradually getting closer to the final shape.

One solution I have considered is to start with a tool diameter that is larger than the actual tool, then minimise this until it is the correct size of the tool.

It could also be done by shallow cuts in depth, progressivly getting deeper.

Is there a way of doing this that doesn't involve lots of GCODE ?

[gar]

071013-0945 EST USA

davejpc:

I do not know what you mean by VTM. I will assume it is a vertical mill. Also I do not know how you are milling a crankshaft on a vertical mill.

Your outline technique is good in my opinion for a number of applications.

Assuming you have subroutine capability, then put the tool path in a subroutine. This eliminate constantly repeating these instructions.

Create a loop that contains the function to change tool diameter in some programmed fashion, and that calls the tool path subroutine.

There are some problems. If at a corner you have a programmed radius of R in the tool path and you make your tool diameter so that its radius is larger then the corner radius, then you should get an execution error.

,

[Geof]

Changing tool diameter with a constant sequence of coordinates called up in a subroutine is how I do it. The one problem is as gar mentions if you make your 'fake' tool diameter for a roughing cutter larger than any concave radius in the sequence you will get an error The way I solve this is to copy the subroutine and take out the corner radii because my machine will do a square corner without complaint. Then I call the modified subroutine for tool diameters larger than the smallest concave radius.

[davejpc]

VTM Vertical Turret Miller I believe, same type as a chester 626 Turret Mill.
Sorry I meant Connecting Rod.
Thanks for the replies, interesting that using the tool diameter seems to be the way to do it.
I presume that there are programs that will take a 2D drawing and convert this to G Code, and also take care of progressively cutting ?

Dave

[Paul_S]

I often use the same tool path for roughing and finishing. The tooling list gives the setup operator the instruction to make the offset for the rougher .01 larger than the rougher's cutter dia.
Example:
(T1 1/2 ROUGHING EM 3 FLT, D1=DIA+.01)
(T2 1/2 EM 3 FLT 1.25 LOC, D2)