How much offset do you get between climb and regular cut.

[knight_toolworks]

I get a fair amount of my prtalpha about .06 this is with a 1/2" bit. not sure if downcut makes it worse or not. it s easy to see on the scrap.
http://i154.photobucket.com/albums/s266/knighttoolworks/posting/3D77003A-B74B-49C6-A3F2-36AC4AB4E2C5_zps1bknv2xk.jpg (http://s154.photobucket.com/user/knighttoolworks/media/posting/3D77003A-B74B-49C6-A3F2-36AC4AB4E2C5_zps1bknv2xk.jpg.html)

[Burkhardt]

Wow, that is a lot. But at which speed, feed and depth does that happen? If it used to be better you may want to check your machine rigidity and backlash with a micrometer and e.g. a luggage or fishing scale. Maybe something is loose or worn?

[knight_toolworks]

oops it is .03 that was using aspires new tool last pass. the offset you choose added that extra. if I cut it as two toolpaths one climb one regular I get about .03

[Ernie Balch]

I have seen similar differences in climb vs conventional final size cuts on slot and tab designs in 3/4 " MDO.
PRS/Alpha 1/4" downcut 2 inch per sec and 12000 RPM

I guess I should to do some measurements on samples before I run another full sheet of MDO because the parts are always slightly oversize or undersize. I think the climb cut gave me oversize parts.

[knight_toolworks]

climb always gives oversized and the sloppiest cuts. after checking I get about .03 oversized. got to play with the aspire last pass tool. I find it is a bit weird if you choose zero offset but opposite direction on the last pass you don't get it. unless you have offset.

[adrianm]

climb always gives oversized and the sloppiest cuts. after checking I get about .03 oversized. got to play with the aspire last pass tool. I find it is a bit weird if you choose zero offset but opposite direction on the last pass you don't get it. unless you have offset.
I would do two toolpaths with the last one the opposite way and then use the merge toolpaths to create one toolpath that cuts each piece entirely.

Even though I always do two toolpaths with the first one offset and the second one correct I don't use the new last pass option as it gives no control over speed or ramping that is different to the first pass. The merge toolpath gives me full control over both passes.

[dlcw]

When cutting with a spiral or compression, I don't use any kind of software offset. The natural effect of the bit being pushed away from the desired cut line gives enough inherent offset that when I do the conventional cut for the final pass, there is enough material left that the cut is super clean. I learned this with eCabs/SBLink about 6 years ago with a large cabinet job I did.

I've looked at parts cut this way and it appears there is probably about .015 offset of the bit because of the climb cut. Just enough for my process of getting a really clean cut. I've also found that if the bits are new, I can go straight from the CNC to the edgebander, the cut is that clean and crisp.

That's my experience. Your mileage may vary.... ;)

[knight_toolworks]

depth of cut is what I noticed about it. but you could set the last pass depth in pass control and that might do it. merge is a good idea. with the last pass option you get each part cut out before going to the next. if you merge what happens when you need to change say the second pass cause something is wonky?

[adrianm]

If you merge by part then each complete part is cut out no matter how many individual toolpaths there are before it moves onto the next.