Re: Flashcut questions

Flashcut does not reconise G40 & G41 the commands for cutter offset off &on.
Although my SW supports tool offset I have always preferred to draw the offset in my cad program. Bobcad does support tool
offset.
Brian. Ont. Canada.

Jon Elson wrote:

> From: Jon Elson <jmelson@...>
>
> "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
>
> ------------------------------------------------------------------------
> Having difficulty getting "in synch" with list members?
> http://www.onelist.com
> Try ONElist's Shared Calendar to organize events, meetings and more!
> ------------------------------------------------------------------------
> welcome to CAD_CAM_EDM_DRO@..., an unmodulated list for the discussion of shop built systems in the above catagories.