Problem... I am trying to cut out several sheets which have drill operations, pockets and of course an outline. On the drill operations it is specified to use the 1/4 comp. tool, but for some reason it wants to drill the holes with the 1/4 comp, then use the 1/8 straight to clean up the hole,which changes the diameter and renders the piece useless. I changed the clean up to 0 and then 4-5 holes later it tries to use the 1/8 straight again. In the DXF there are 2 different diameter holes to be drilled. One is .28 and the other is approximately 1 inch. In my tool settings I do not have the 1/8 straight selected for drill operations, only the pocket is selected, why would the program be wanting to use 1/8" straight to drill a 1" diamet hole. Now I could eliminate the 1/8, except I need it in use to pocket the text that are being cut to .0625. Any suggestions?? I mean basically right now my questions are:
1) In the DXF the layer for holes that need to be cut is labeled drill, but on the super controller it is showing pocket/rout, why?
2) Does the program always want to clean up the holes in a drill operation?
Matt "ineedhelp"
DXF Clean Up tool Problem
Moderators: Jason Susnjara, Larry Epplin, Clint Buechlein, Jim Bullis
-
Matt Adams
- New Member
- Posts: 2
- Joined: Fri, May 25 2012, 1:41PM
- Company Name: Central City Millworks
- Country: UNITED STATES
- Location: New Orleans, LA
-
Daniel Odom
- Senior Member
- Posts: 204
- Joined: Thu, Oct 20 2011, 12:52PM
- Company Name: Carlton Kitchen and Bath
- Country: UNITED STATES
Re: DXF Clean Up tool Problem
Post the file you're having trouble with. Check your tool tolerance in the tool settings of control nesting, see if any tools are set to interpolate also.
-
Daniel Vonderheide
- Thermwood Team
- Posts: 361
- Joined: Wed, May 17 2006, 11:25AM
- Location: Thermwood
Re: DXF Clean Up tool Problem
When Control Nesting is given an operation it checks the tooling list starting with the operation 1 tool then going down the list until it finds a tool it can use. If it goes through the operations list and does not find a tool it can use, it then passes the operation to the pocketing routine. This is what is happening in your part. Most likely what is happening is that your 1/4 tool does not measure .25 in your tool management and your tolerance is set to .001. This is keeping CN from selecting this tool. The other thing to look at is if the 1/4 tool is set to interpolate, and if so, what is the diameter you are allowingit to interpolate to? If you set the 1/4 tool to interpolate 1 inch, then it will not pocket the drill holes.
-
Matt Adams
- New Member
- Posts: 2
- Joined: Fri, May 25 2012, 1:41PM
- Company Name: Central City Millworks
- Country: UNITED STATES
- Location: New Orleans, LA
Re: DXF Clean Up tool Problem
Thank you for the replies. I finally got it figured out after reading your posts. It was a tool diameter vs. layer name. my 1/8 straight was set up as .124 and was actually .127 so after changing the setting and 0ing out the clean up, everything is working fine now. Of course that was after messing up one sheet but at least I know for the next time...
