Can't find an approapriate tool

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

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

User avatar
Dale Wills
Senior Member
Posts: 190
Joined: Mon, Oct 10 2005, 11:09PM
Company Name: none
Country: AUSTRALIA
Location: Camperdown, Victoria, Australia

Can't find an approapriate tool

Postby Dale Wills » Tue, Dec 08 2009, 12:05AM

A friend is trying to machine some 25mm board. This job has blind dados and when nesting they are getting an error saying 'can't find approapriate tool between 12.7mm and 25.3mm. I forget how to fix this. I think it has something to do with the depth of the dado as apposed to the diameter of the cutter. What do they have to change to get this to work?
Thanks

Ryan Hochgesang

Re: Can't find an approapriate tool

Postby Ryan Hochgesang » Tue, Dec 08 2009, 8:21AM

Dale,

This error is typically caused by a tool not being setup in tooling, which will fit a particular hole, dado or pocket. You may also need to open up your Select Tolerance, which is located under TOOLING. This will help select a tool that is close, but may not have the exact dia. that CN is searching for.

User avatar
Dale Wills
Senior Member
Posts: 190
Joined: Mon, Oct 10 2005, 11:09PM
Company Name: none
Country: AUSTRALIA
Location: Camperdown, Victoria, Australia

Re: Can't find an approapriate tool

Postby Dale Wills » Tue, Dec 08 2009, 5:56PM

There are various tools that are set to perform these operations (6mm, 10mm). But why does it need something larger than 12.7 to perform this 25mm wide dado ?? 12.7mm happens to be half the width of the dado being machined. When a dado is being machined do they only machine up and back once or are they able to complete many passes to complete a dado such as 25mm wide? I can't see why a 10mm tool can't perforn this dado by making 3 passes.
Dale

User avatar
Paul Ford
eCabinets Beta Tester
Posts: 632
Joined: Wed, May 18 2005, 1:18AM
Location: Rotorua - NewZealand
Contact:

Re: Can't find an approapriate tool

Postby Paul Ford » Wed, Dec 09 2009, 12:55AM

Hi Dale,
The way the tooling works for Dado's is the tool needs to be at least half the diameter of the dado cut itself which in this case is 12.7mm. CN will only do 2 passes for a dado cut. It may look like it's doing 3 passes but that's just because it starts in the middle of the dado so it can ramp in.

I just had another though. You say your Dado is 25mm wide... If you go in to the settings for this cabinet in eCabinets, does is state that the dado is 25mm wide? You're obviously using 25mm thick material but you will find under your construction parameters that it allows for a Fit Clearance, your dado could infact be 25.5mm wide...
Hope this helps
Paul

Ryan Hochgesang

Re: Can't find an approapriate tool

Postby Ryan Hochgesang » Wed, Dec 09 2009, 10:13AM

In addition to the note, that the tool dia. must be able to cut a dado in two passes, you will also need to know that your pocket tool setup will be used for all cuts which are created in the PART editor. If you continue to have issues with tooling selection, you can sent a copy of the related files to our support email address (program@thermwood.com) and we will have a look. For us to look at your issue in greater detail, we will need to have a copy of your EXPORT file from Control Nesting along with the design file (ie: .hsf, .esa or .dxf).

Rob Davis
Guru Member
Posts: 316
Joined: Mon, May 23 2005, 5:43PM
Location: Indiana
Contact:

Re: Can't find an approapriate tool

Postby Rob Davis » Wed, Dec 09 2009, 3:47PM

I don't have this problem but just want clarification of what I think I am understanding by reading this thread.
"All cuts in Part Editor are done with the pocket tool." ? Is this really true? When we make part editor cuts to the outline of parts as we often do, these cuts are made by the outline tool, which is not necessarily the same as the pocket tool. Correct? Our actual experience is yes.
Second, if the above statement is true at face value, then do I need to make certain that my part editor cuts are at least as big as one half the width of the largest pocket? For example, if I want to add a part editor cut for metal track shelf brackets (.625" wide), but my pocket tool is set to 0.25, will I have a problem or will it do this in multiple passes? Or conversely, if I want to make a .375" part editor cut but my pocket tool is set to .5", it won't go get a smaller tool and perform this operation?
Just trying to clarify my understanding of the above explanation. Perhaps my brain is muddy (often the case) but I want to understand before I create a situation I can't perform.
Thanks in advance for the answer, if there is one.

Ryan Hochgesang

Re: Can't find an approapriate tool

Postby Ryan Hochgesang » Wed, Dec 09 2009, 5:03PM

Perhaps I should reword my last posting...... I was implying that all interior cuts created in the Part editor will be performed using a tool from pocket tool list. The outline or profile of part will still use the outline tool that is setup in TOOLING.

As far as your second question, you do not have to worry about the twice dia. of tool rule used with dados, when cutting a pocket. Pocket geom. can be cut by spiral or zigzag so the tool can clean out the entire area within perimeter of pocket design. Your example of .25 tool for a .625 pocket should be good to go. As far as pocket smaller than tool, CN 5.48 now allows you to setup multiple pocket tools so you can be sure to set a range of tools that will work for your pocketing operations.

Just let me know if you have any further questions or concerns, sorry about any confusion I may have caused with previous post.


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: No registered users and 7 guests