Rebates with lip cutouts

[jason galbraith]

I need to know, because I've come across this situation so many times. I am doing a through cut in a piece of 32mm and then it has an11mm lip that a piece of board sits on the through cut is fine, but the router then wants to hog out the whole centre section to leave me with the 11mm lip. Is there a way to just get it to do the outline where the 11mm lip is. It will leave me a reasonable off cut and save a lot of machine time. I think this is possible with a .dxf? if so could anyone pretty please do me a template that I can then use to get my head around and see how it works, then I can change it to suit my needs. Or if it is possible through ecabs some how that would be awesome. My trick at the moment is to do two files with both items set as cut throughs and then change the height of the bit in the machine to fool it.

[Daniel Odom]

Use the profile modeler in ecabinets instead of pocket.

[Josh Rayburn]

Jason,
You can do this with a single pass in the profile modeler if you have your profile tools set up correctly, but that will suit you only up to two passes, i.e. two "profiles". A dxf file would make it much simpler and faster.
Start with a rectangle on the outline layer, then you can add geometry to comp in or comp out as desired. The layer name will indicate the compensation and the depth of the cut. Check in the control nesting manual under dxf files for a good explanation on this.
jnr

[Kerry Fullington]

Jason,

If you will cut out the centers using geometry or Closed Contour you can then profile the inside edge with a tool you created to cut the rabbet. Make sure you set up the correct tool in the Profile Modeler for the rabbet cut. This way you can still nest the parts and there is no need for a secondary operation or a .dxf

Kerry

[jason galbraith]

Thanks for the replies. I tried Kerrys method as it seems easiest for me and it sort of worked. It did the through cut and then picked the 6mm bit out and proceded to to do the rebate part at about 5 inches per minute and went down in just over .5mm increments. ( about 26 steps to get down 13mm in thickness) needless to say it took a long time. What settings should I be looking at in my machine to
A) get it to choose the right bit ( not as important the 6mm was fine)?
B) Get it to do the rebate quickly with maybe at most 2 step down increments?

Thanks again

[Kerry Fullington]

Jason,

In Profile Modeler set up a tool group that only has a single tool that will cut the rebate in one pass. (I use a 1/2") and only that tool. Set that tool as the Custom Tool also. Make that tool group the default in Profile modeler and now that will be the only tool available for the operation and should make the cut in one pass.
Make sure you set up this tool to cut deep enough in Profile Modeler so that it will cut the depth in one pass. Profile cuts use the tool settings in Profile Modeler not Control Nesting
Profile Modeler is modeling the rebate with the 6mm tool now which is why it makes multiple passes.

[jason galbraith]

Thanks very much for that Kerry. All sorted out now and working as it should be. Cheers

[Sean O' Hare]

Jason,

when I need a rebate beside a cut-out, I offset it .1mm. That way, the machine cuts them separately with the standard tools.

Sean