Re: Flashcut questions

"Ian W. Wright" wrote:

> From: "Ian W. Wright" <Ian@...>
>
> Hi,
>
> I downloaded an evaluation copy of Flashcut which I have been looking at
> today and a couple of questions have come to mind which I'm sure someone
> can answer.
>
> I cannot see any way to make the programme take account of tool offsets
> - i.e. the allowance for the diameter of the milling cutter. Is this not
> one of its functions and, if not, how do users get around the problem
> (if such it is - I've never yet quite managed to understand how the
> programmes which do use tool offset corrections decide which side of a
> line they should cut on ).

I can't answer as far as flashcut is concerned, but there are RS-274D
modal commands that specify 'cutter left of part' or 'cutter right of part'.
In Bobcad/CAM, they really don't quite support this, either. They
do have a function that 'offsets' a toolpath from the actual part outline
on the drawing. This can be used for leaving a finish allowance on the
part when roughing, as well as offsetting the tool by its radius.

> Do you have to decide on the exact size of
> cutter before drawing the component in CAD and draw the cutter path
> rather than the component?

Yes, to do things this way, you would need to know the tool size in
advance. Very messy, and not compatible with using reground
tools in the shop.

Now, you can make the program produce a toolpath that follows
the actual part outline. You have to be careful to radius all inside
corners to greater than the expected tool radius. Then, you can manually
place a lead-in and lead-out for the radius compensation as you
specify the direction, etc. to follow when cutting the part. Then,
you manually edit into the CAM-produced RS-274D file the commands
to enter radius compensation and exit at the end. Finally, you
do a test cut on the machine (or a CAM previewer, but I don't
have one that supports this) to see if you specified the correct
side of the part. I made a tool which has a spring-loaded ballpoint
pen cartridge in a 1/2" rod. I put this in a collet and set the Z so
that it will touch the pen to a piece of paper taped to a 'platen'
held in the vise, when the tool is lowered to the workpiece.
It then draws the centerline of the toolpath, so you can see
whether it is doing what you want. Actually, the way I do
this is to first set the tool radius to zero, such that the drawing
shows the actual part outline. Then, I set the tool radius to
the correct value for the tool I'll be using, and run the program
again. If the side of the part has been specified correctly,
you get a new line that follows completely around the outside of
the part by the desired radius. If not, it will do the inside, but
the lead-in and lead-out points will not be well chosen for
doing the inside.

One other trick I use, especially when typing in a G-code program
without benefit of CAD/CAM, is to enter into the tool table a larger tool
diameter/radius that the tool actually is. This makes the machine
make a roughing pass, leaving extra material on the part.
Then, you reduce the oversize specification, and run it again, and
it takes off some of that excess. Finally, setting the tool table
to the actual tool size gives a finish pass, cutting the part to
the desired dimensions.

All of the above pertains to my particular combination of CAD/CAM
and CNC control, of course, but should be fairly general.

>
> Secondly, The programme ignores any 'Z' component when it is importing
> from a DXF file - is this just a limitation on the demo version or is
> the programme only really intended for 2 1/2D engraving etc.? I
> suspect not as you can enter 'Z' amounts manually to the G-code and it
> will emulate cutting them.

Many of the low-cost CAD/CAM programs are really 2-D programs,
with assorted hacks to let them perform 3-D work. Some of these hacks
are quite awful, and you really are quite limited by them. Others do a
bit better, but they still are cumbersome.

Jon