Tooling Error

Discuss Thermwood 3-axis Machinery, Controller, and Software.

Moderators: Jason Susnjara, Larry Epplin, Clint Buechlein, Rich Kasten

User avatar
Damon Nabors
eCabinets Beta Tester
Posts: 923
Joined: Wed, Apr 05 2006, 5:50PM
Location: Marion, Ar.
Contact:

Tooling Error

Postby Damon Nabors » Thu, Nov 22 2007, 7:22PM

I loaded the file and nested the file, clicked WRITE CNC, then it comes up with a tool error. I scrolled down the file to the error and it said something about .....tool diameter .375 not found (Something to that effect). I have a 3/8 compression bit loaded in the tool holder and it is set in the settings to dado/rout, drill,..... and so forth. The tool diameter is set up at .3665. I do not understand why I have the error because .3665 is smaller than the .375 tool requirment.


Can someone shed some lite on this problem. :?:

Thanks,
Damon

Joe Soto
Guru Member
Posts: 351
Joined: Thu, May 19 2005, 7:50PM
Company Name: Fancyridge Wood Products LLC
Location: Greensburg, Ky

Postby Joe Soto » Thu, Nov 22 2007, 7:36PM

Damon, I'm not at the control so I am going from memory. On the tooling page of control nesting there is a setting for tool tolerance, check to see if set too tight. Joe

Rob Frenette
Junior Member
Posts: 73
Joined: Thu, Nov 17 2005, 8:19PM
Location: Calgary, Alberta, Canada

Postby Rob Frenette » Thu, Nov 22 2007, 9:58PM

Damon, was this an error for a rout/dado operation? If so, why are you using a compression? We normally use a down cut for this. Usually when you get this kind of error its normally to do with rout or dado operations.
Maybe you give some more details as to what kind of machining you are doing and what thickness of material you are cutting. Rob
Rob Frenette
_______________

Calmark Cabinetry & Woodwork Ltd
Specializing in CNC Machining & Edgebanding

Forrest Chapman
eCabinets Beta Tester
Posts: 1160
Joined: Mon, May 30 2005, 2:26PM
Location: Anderson SC.
Contact:

Postby Forrest Chapman » Thu, Nov 22 2007, 10:23PM

Damon,

If the error read cannot find tool between .375 and .75 then you will need a tool larger than .375 but smaller than .75\". This is probably due to a full dado somewhere. Scroll down and find the error to locate the sheet and part number then you can tell what operation it is attempting.


Forrest

Mark Hesketh
Guru Member
Posts: 366
Joined: Fri, Aug 25 2006, 9:12AM
Company Name: Paris Kitchens
Country: CANADA
Location: Paris, ontario

Postby Mark Hesketh » Fri, Nov 23 2007, 7:16AM

is this a dxf file that you are trying to cut? I'm pretty sure that when you set your layer names for different opperations in autocad, you need to specify not only the depth of the opperation, but the diameter of the tool that is doing it. If you set the wrong diameter of tool, it won't be able to run because that is the only diameter it wants to use. I think the outline layer is the only one that will pick up the tool diameter from the machine. I have run into this problem alot when getting files from others to cut.

Joe Soto
Guru Member
Posts: 351
Joined: Thu, May 19 2005, 7:50PM
Company Name: Fancyridge Wood Products LLC
Location: Greensburg, Ky

Postby Joe Soto » Fri, Nov 23 2007, 7:31AM

Damon, What Forrest is saying is if you have a .3665 bit it cannot cut a .75 dado in two passes (.3665*2= .733). This may be your problem.
What I was referring to was calling for a tool size in a .dxf. Control nesting will look for that size only, unless you have your tolerance set up and have a cutter within that range.
Here is a quote from an old CN update that explains it better,
Set tool tolerance. This value can be set in Tooling. This value will tell Control Nesting what tolerance to use when selecting the proper tool for an operation. The tolerance value is applied to the diameter of the tool. For example, if an operation calls for a tool with a diameter of 0.25\" and the tool at the control that will work for this operation is actually 0.245 a tolerance of 0.006\" will allow this tool to be selected for the operation.
(ADDED)
Joe

User avatar
Damon Nabors
eCabinets Beta Tester
Posts: 923
Joined: Wed, Apr 05 2006, 5:50PM
Location: Marion, Ar.
Contact:

Postby Damon Nabors » Fri, Nov 23 2007, 8:51AM

I was not cutting a full dado, I was making a tooling cabinet to hold my tool holders and bits. It has a series of holes ranging from 1/2 down to 3/16 drilled .375 deep into one of the shelves so the bits can slip down into the holes. I made each hole .005 larger to make sure they where not too tight. Other than the holes, it was a standard cabinet with blind dado's. I am going to run the program again and write down exactly what the error message said and re-post.

Thanks for your help.

Damon
Attachments
tool holder cabinet.jpg
tool holder cabinet.jpg (17.27 KiB) Viewed 5115 times

User avatar
Damon Nabors
eCabinets Beta Tester
Posts: 923
Joined: Wed, Apr 05 2006, 5:50PM
Location: Marion, Ar.
Contact:

Postby Damon Nabors » Fri, Nov 23 2007, 9:21AM

Ok, when I load the program, It pops up with:\"There was a problem finding an appropriate tool for an operation, Please check the cnc file......\"

I then scrolled down untill I get to sheet 1, part 5,...
\"error: tool size: 0.375 not setup in tooling (pocket clean up)

I do have a .375 tool set up but it mics out at .3665. If I am at the screen where you select NEST, TOOLING, WRITE CNC, ......If I click the tooling icon, tool .375 has a tolerance of .001.

If you look at the Deck of the cabinet, I cut a 1/8\" pocket 2.27\" in diameter, and a through cut in the center of the pocket 1.27\".

If I go to my tool setup screen and change the diameter of the tool from .3665 to .375, the program runs ok, but I have an incorrect actual tool diameter.


Damon

Joe Soto
Guru Member
Posts: 351
Joined: Thu, May 19 2005, 7:50PM
Company Name: Fancyridge Wood Products LLC
Location: Greensburg, Ky

Postby Joe Soto » Fri, Nov 23 2007, 9:31AM

I do have a .375 tool set up but it mics out at .3665. If I am at the screen where you select NEST, TOOLING, WRITE CNC, ......If I click the tooling icon, tool .375 has a tolerance of .001.

Try .0085

Mark Hesketh
Guru Member
Posts: 366
Joined: Fri, Aug 25 2006, 9:12AM
Company Name: Paris Kitchens
Country: CANADA
Location: Paris, ontario

Postby Mark Hesketh » Fri, Nov 23 2007, 9:31AM

make sure that you have your tools set to interpolate, and that the interpolate diameter is sufficiently large enough to be able to run through the holes you are making. That's if it's the holes causing the problems and not the dadoes.

Do you have your 3/8 bit set up as your pocketing tool in the settings dialogue? If you do, you need to manually change the diameter setting for that... it might be looking for your pocketing tool to run the blind dadoes.

User avatar
Damon Nabors
eCabinets Beta Tester
Posts: 923
Joined: Wed, Apr 05 2006, 5:50PM
Location: Marion, Ar.
Contact:

Postby Damon Nabors » Fri, Nov 23 2007, 10:26AM

the pocketing tool is also set up as .375. I change the INTERPOLATE max diameter to 2.5 from 2 and it did not give me the error code this time. But when I nest the parts the pocket cuts on the screen are much larger. Will this create a problem???? I can not find anything in the Manual about Interplation settings.

Joe Soto
Guru Member
Posts: 351
Joined: Thu, May 19 2005, 7:50PM
Company Name: Fancyridge Wood Products LLC
Location: Greensburg, Ky

Postby Joe Soto » Fri, Nov 23 2007, 10:48AM

Sometimes this happens on the screen, nest just the one part, write cnc the f3 f6 to graph it then zoom in. Or you could dry run it above the part. I just change the wasteboard thickness

Forrest Chapman
eCabinets Beta Tester
Posts: 1160
Joined: Mon, May 30 2005, 2:26PM
Location: Anderson SC.
Contact:

Postby Forrest Chapman » Fri, Nov 23 2007, 6:57PM

The pocket tool setting has to match the size of the desired tool .3665

User avatar
Damon Nabors
eCabinets Beta Tester
Posts: 923
Joined: Wed, Apr 05 2006, 5:50PM
Location: Marion, Ar.
Contact:

Postby Damon Nabors » Sat, Nov 24 2007, 11:01PM

Forrest, I had the pocket tool set at .375 instead of .3665. That fixed the problem. Thanks a million for your help

Damon


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: No registered users and 6 guests