Can someone tell me if with the newest build of carbide create there is a better way to design a toolpath regarding the retract height of doing a pocket and then v-carve? The project is cutting four circle coasters from one piece of 0.500" stock, each with a 0.250" pocket and a v-carve engraving on the pocket bottom. Currently I’ve split it into two toolpaths to allow for rezeroing after the tool change between endmill and vee bit (I do not own a bitsetter).
Toolpath 1 (Endmill) - Zero height set to stock bottom (wasteboard). Pocket toolpath cuts the 1/4" pocket (0.000" to 0.250" depth) and contour (0.000" to 0.500" max depth) for each of the four circle coasters
Toolpath 2 (Vee) - Zero height set to stock top but is zeroed on the machine to the bottom of the pocket. The retract height is set to 0.300" to raise above the pocket height when moving from one coaster to the next. V-carve toolpath cuts the engraving (0.000" to 0.500" max depth) for each of the four shapes
The v-carve toolpath is slow because it’s constantly retracting to the 0.300" height even when cutting within the pocket. Looking at older posts it seemed like that was a known limitation of the software and there were workarounds to clean up the gcode files after they were saved. I was curious to know if the newer versions of the software can now account for these repositioning steps on it’s own if designed the right way. The simulated toolpaths I’ve attempted do not seem to show what I would expect to look like two different retract heights.
There is no possibility to have a custom retract height per toolpath (that I know of), short of editing the Gcode file manually (tedious…and error prone).
If your four coasters are always in the same location, a workaround could be to only run on vcarve job on one coaster at a time (with small retract height, as it won’t be moving to another coaster), then move to the next coaster, reset zero, re-run vcarve file there. If you make a note of where the zeroing points are for each coaster, moving from one to the other and rezeroing is a matter of a few seconds.
To further streamline this you could utilize GRBL’s work offsets feature, to memorize the four zero references in advance, and switch from one to the other with a single command.
Unfortunately sometimes the workarounds are as time consuming as just letting the machine just run. If you calculate the time required to modify your CC file and the anxiety of waiting to see if it works just let it go and the machine will take as long as it takes. After all you said you only had 4 to make. If you start a production run then it would be worthwhile to make changes because of the incremental time savings that add up over time and quantity.
@gdon_2003 I agree that sometimes it’s better to be patient rather than trying to find a shortcut. However this is actually for a production run and I’m making about 160 total it’s just that the lumber stock I have access to makes it so they fit four to a board. If there’s a better way to do it I’m always wanting to learn and it would have a noticeable impact on time/quantity in the long run.
@Julien essentially what I’m taking from your comment is breaking them into four smaller toolpaths to avoid the movement from one coaster to the next is about my only option. The coasters are always in the same location so rather than having to reset the zero for all four positions is there a way to force a pause step (e.g. a tool change) to make the machine fully retract? Then I could just click through the prompts quickly to move on to the next coasters. The tool change wouldn’t actually be a change to the machine, only in the design I could have four identical bits with different names assigned to the four coasters so it “thinks” I’m changing and therefore pauses the run.
Interesting approach. Since CC only has one retract height setting, you would need to create the four vcarve toolpaths in a different c2d file. Then you could indeed fake tool changes by using multiple tool definition for the same tool. I can’t remember what CC’s generated G-code behavior is when combining multiple toolpaths into a single file while NOT having the bitsetter enabled. I know it stops and waits for a “tool change”, with no possibility to jog (which usually make this useless), but I can’t remember at which height it parks during that pause. If it pauses “high enough” (to clear the highest part of the stock), this might work. I’m afraid it just parks at retract height, which would be the small/vcarve one in your case, so no luck. The easiest is probably to try, and run it as an air job to verify?
If for some reason this does not work, the work offset trick would boil down to typing one line in the MDI console and click start. Not quite as fast as just discarding a prompt, but close.
For anybody interested the fake tool change approach did work. I created four separate toolpaths with differently named tools (but identical bit information). When the machine finished the first toolpath it parks at the retract height and prompts to turn off the router. Clicking resume it then raises to full height and prompts to change the tools. Clicking resume again it prompts to turn on the router and then begins the second toolpath, moving at a safe height above the material.
darn, I was just running into the issue as well, got the tool paths all done for a 2 sided valet tray (about an hour total) and then added in the vcarve to the inside of the dish and it added a whopping 32 hours to the tool path time. (likely 95% of it is retract moves)