Resetting Control Nesting settings

[Brent Riley]

Is there any way to retrieve the tool settings from previous settings? I might have erased all the tools with the erase button now I'm unsure of which ones to put back in. I'm only using a 10mm Triple flute cutter as an outline tool and same as for any dado or pocketing. The Drill banks are also used.

I tried to enter only the 10mm in and the drill banks but still come up with the problem.

Every time I go to nest I get Couldn't find tool to work for pocket operation "#" on * end , top end etc. This is up to 400 times before it ends in either an incomplete looking nest, or another error once pocketing has been finished saying Error Opening Nestlib. Exiting...

Im using the default nesting group, 10mm cutter as outline tool.

How many of the operational tools need to be set?

There are 50 tool selection areas. do I need to enter all the tools. I use a 10mm triple flute cutter for outline and pocketing and all the secondary actuator drill banks.

I have been nesting everything and cutting all the cabinets previously. Now I seem to me missing a lot of settings as I cant nest any jobs in the 91000 super control without getting "Couldn't find tool to work for pocket operation 1 on left end"

right through every job until its been up to 400+ and naming every piece. Even a simple 400mm cabinet. Jobs cut previously are now not nesting either.

It seems to be a problem converting the TWD to a CNC file. Iver checked the CNC files I do manage to create and they say error missing a tool.

[Daniel Odom]

Maybe do a system restore or re-install control nesting would be my best guess. I always re-install control nesting whenever things get really weird without an apparent reason. I'd try and contact thermwood first though, the nestlib thing doesn't sound right, tool error is pretty normal if you don't have the tools set up correctly.

Not sure about your specific machine but on mine you don't need to set up all 50 of the tool groups, just default. The others are optional if you want to use different settings for different materials. You need a tool for every possible operation contained in your file that you're trying to process or you'll prob. get an error, tool diameter tolerance can also play a role in this. You need an outline tool and then a tool for dado, pocketing, drilling and maybe interpolating. You can use the same tool for outline and dado/pocket but you still have to select it for outline and then select it again below for any secondary operation you want to use it for. I don't see an option for pocketing from your screenshots, not sure if that's b/c your software is older than mine? I know one time I had a problem with pocketing and it turned out that I had my pocket step-over % value formatted as .70 rather than 70 and it took me a while to figure out what was going on. Sometimes it's just one funked up parameter that screws up everything. I don't have a drill bank so I can't help you there. Maybe try flipping through the manual I think it should cover most of what you need to know.

[Brent Riley]

Thanks Daniel, unfortunately im a long way from USA. I will try a few settings and try reinstall the control nesting.

Hopefully there is an archive for the nesting program installer. Not sure upgrading software before an important job is worth the risk until Ive run out of options.

[Josh Rayburn]

Brent,
In control nesting, under the file menu, there are two options: save settings/tooling, and load settings/tooling. Once you have the settings you want, including everything on the tooling setup and the settings pages, these can be saved as a .cst file. Then that file can be loaded at any time to get you back to "ground zero". You can even use this feature to save a certain group of settings for a certain job if it's a bear to set up. This way if you had to renest something or even recut a part, you could simply load the .cst file that you created for that job, and then enter your recut number, and off you go.

The pocket operation error is almost always due to a "pocket" which is smaller than all of your pocketing tools. Make sure you know what size pockets need to be cut, and then be sure you have a tool (doesn't matter where in the operations list) set up that is at least .002" smaller than the pocket. That tool must be checked for pocketing.
If you open the .cnc file after you see an error, and run a search for "error" then it will actually say in the code that it couldn't find a tool between x size and y size which will indicate what size tool you need to load and select for pocketing.

You do not need to enter any particular number of tools in the operations list.
Hope this helps.
jnr