jimwill2 wrote:Why not just layout individual lines that will create your parts? If you aren't using a vacuum bed you can leave a little "onion skin" to hold your sheet together.
tomgardiner wrote:There is no automatic way to layout a common cut line in V-Carve. For files that will be used repeatedly you can spend the time to layout your parts with the same width or height in a grid. You can drag a rectangle by a corner and snap to its neighbor. Pressing the M key will bring up the move function and a relative move will space the parts by the bit dimension.
You can optimize the cuts by node editing (N on the keyboard) changing the start point will reduce the non cut travel. In the toolpath settings check the box always use start points. If the advanced settings option is checked you can choose from the Order tab - vector selection order.
If other operations are being done to the parts be careful not to disturb the other elements associated with those parts as you move them around. You can group a selection quickly by keying G ungroup U.
That is a start
martin54 wrote:Nothing to do with your cutting question, more about your choice of machine. If you are operating in a production enviroment would you not be better off with a bigger machine? The size you have mentioned to me would produce a lot of waste material unless you only intend to use it for one specific job. I don't do prouction work but have done jobs where I wish the machine I had would take a full sheet so I could make better use of my material when cutting multiples from sheet materials.
Adrian wrote:You might struggle with the corners with that type of board with common line cutting. It was a few years ago now but I had a contract to cut lots for a wood stove manufacturer and it was incredibly easy to break the corners while cutting if the bit was putting pressure on the finished part rather than the waste. It's easier to play around with conventional/climb cutting when each part has its "own" vector.
Adrian wrote:I started off using a 6mm two flute spiral down cutter running at 11000rpm with a feed rate of 400ipm with the pass depth set to be 1 pass but with a spiral ramp set. I didn't experiment that much with the feed rates as the material didn't give the sort of feedback you would get from a normal wood material so it was hard to dial it in exactly.
I didn't use a vacuum hold down with these as I generally find I don't need it with materials over 10mm or so thickness and a reasonable amount of weight. You could probably dispense with the spiral ramp with a vacuum hold down.