Tool Diameter

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

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

Dave Burtchell
Junior Member
Posts: 98
Joined: Thu, Jun 30 2005, 10:04PM

Tool Diameter

Postby Dave Burtchell » Tue, Aug 08 2006, 4:16PM

Hi,

The office sends out .dxf files with d0p375 for my outline/dado/centerline tool. The tool is not always .375, latest one is .372. This isn't a problem most of the time, but today I was making some jigs that had to be dead on. Any way to fudge the tool dia at the machine? Something in settings would be nice.

Thanks,
Dave

User avatar
Bill Rutherford
eCabinets Beta Tester
Posts: 386
Joined: Tue, May 10 2005, 5:23AM
Location: Lancaster, NH
Contact:

Postby Bill Rutherford » Wed, Aug 09 2006, 5:15AM

Dave,
A diameter change in the tool table (F9-F2) will not adversly effect outline or dado operations. The control will automatically compensate for the diameter you have plugged in, in fact we use this on a regular basis to tweak fits. The centerline tool is a different story, here rolling nest is looking for an exact size tool. The only way around this I can think of is to set the tool for .375, nest the parts, write cnc and then change the tool back to its actual diameter. The down side here is that since I don't think there is any cutter comp on a centerline operation, the machine will run the part as though the bit is .375 not .372 Hope this helps some
Bill Rutherford
North Woods Manufacturing
Full service CNC Machining
and Edge Banding
http://www.northwoodsmanufacturing.com

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Tool Diameter

Postby Brad McIntosh » Mon, Aug 14 2006, 9:06PM

What would make Control Nestings handling of DXF files even more amazing would be the following:

In the Tool Table (Tool Manager) -

1. Have a field for the \"theoretical\" tool diameter. So, a 1/2\" tool would be 0.500. (Sharpened or not. It reflects what it is *suppose* to be or originally was.)

2. Have a field for the \"actual\" tool diameter. Here, the above tool would be 0.500 if NEW or would reflect the \"actual\" diameter if it has been sharpened. ** There should be a built-in limitation to how much smaller the \"actual\" tool could be in comparison to the \"theoretical\" tool diameter. (It should be the same size or smaller, perhaps the difference limited to a a percentage of the NEW or \"theroetical\" tool's diameter.) This would ensure that when pocketing, the passes still overlap.

With the two parameters above, the DXF \"programmer\" could specify the \"theoretical\" tool diameter for such operations as pockets, chains, etc. on the layer name. Control Nesting in turn would search for the \"theoretical\" tool diameter that matched the diameter specified on the layer name when selecting the tool to use, but the resulting tool comp codes in the output would use the \"actual\" tool diameter to perform the radius offset when cutting.

With the above in place, DXF files could be prepared without any fore-knowledge of the tools' \"actual\" diameters. (No more editing the DXF to change the D specification to match a sharpened 1/2\" cutter that is now 0.485 !)

Just a thought...

User avatar
Bill Rutherford
eCabinets Beta Tester
Posts: 386
Joined: Tue, May 10 2005, 5:23AM
Location: Lancaster, NH
Contact:

Postby Bill Rutherford » Tue, Aug 15 2006, 6:17AM

Nice idea Brad, I think that would definetley help. Another possibility that would add even more flexibility for the programmer is instead of having the layer name specify tool diameter, have it specify tool number. That way I could have three different 1/2\" diameter bits set up for that material and control exactly which bit RN called to make the pocket. (maybe a 1/2\" mortise compression for \"drilling\" large diameter deep holes and for deep dados, a 1/2\" downspiral for a shallow pocket, and a 1/2\" compression for cutting the perimeter (assuming a thick piece, not standard 3/4)
Bill Rutherford

North Woods Manufacturing

Full service CNC Machining

and Edge Banding

http://www.northwoodsmanufacturing.com

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Tool Diameter

Postby Brad McIntosh » Tue, Aug 15 2006, 6:57AM

Bill,

There is a VERY GOOD reason why tool numbers are defined on the layer names. By NOT defining actual tool numbers, the DXF files are not suppose to be \"machine specific\". That is to say that, the DXF can be sent to ANY machine, as long as the tools with any specified diameters that may be defined within the file exist on the machine. (Non-specified ones are just automatically used.)

The general concept was originally for eCabinets itself. By beingNON-TOOL-NUMBER_SPECIFIC (including any profiles), virtually ANY machine with tooling that would fit into the \"spaces\" defined for the Holes, Dadoes, Cut-Outs and Pockets could machine the parts. Of course, profiles could be defined/assigned, either for a feature using a specific tool or for a group of generic \"modeling tools\" at the machine via the Profile Modeler. So as far as eCab is concerned, not even a tool diameter is needed to be specified.

This concept has been extended as much as possible to the Layered DXF files. Tool diameter specifications were added only due to the nature of some of the operations - but againl the \"tool number specification\" has been left out in order to try and keep the DXF machinable on ANY machine, regardless of how the tools are actually setup/numbered at the machine.

Of course, having to know the EXACT diameter of a tool as it exists on a specific machine kind of puts a small snag in this \"universality\" of some of these layer definitions. But that is why I suggested the \"theoretical\" and \"actual\" tool diameter definitions in Tool Manager. This will still keep the concept NON-TOOL-NUMBER SEPECFIC and even more NON-MACHINE-SPECIFIC than it sometimes is now.

(Clear as mud?? :roll: :D )

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Tool Specifications

Postby Brad McIntosh » Tue, Aug 15 2006, 7:10AM

Bill,

After reading your post a second time, it triggered another idea that I had had.. (I'll try and be short this time! haha)

What if within Tool Manager, not only would we define the \"theoretical\" and \"actual\" tool diameters (for my first idea), but also a general description of the tool geometry?

This would not nessecarily be a \"drawing\" of the profile of the tool, but more general like: UPSHEAR, DOWNSHEAR, COMPRESSION

With these qualifiers, Control Nesting could make better \"automatic\" tool selections. A NON-THRU Pocket, Dado or similar operation would llok for a Downshear tool that meets the diameter specification required. Whereas Thru-Operation would put a priority on a Compression (up/downshear) tool. I am sure that something could be worked out if drill types also had specific operation/geometry characteristics. :?:

Whad'ya think?

User avatar
Bill Rutherford
eCabinets Beta Tester
Posts: 386
Joined: Tue, May 10 2005, 5:23AM
Location: Lancaster, NH
Contact:

Postby Bill Rutherford » Tue, Aug 15 2006, 7:37AM

Brad,
Your idea would work as well. As far as DXF files not being machine specific, I see your point, but the file would still basically be generic with only a minor amount of tweaking and even then only when that specific command was called perhaps something like this.

Pocket z0p375 D0p375 would look for a .375 tool or
pocket z0p375 tool2 would force it to call tool 2

giving the operator total flexibility, if the part is a generic part use the first command, if it a programmer programming for a specific machine (as is often the case) he can force a specific tool just like in MasterCam. Actually I could see this carrying to outlines and drills as well. There are times when due to our large database of tools and materials maybe 2 different tools would work for the same operation but due to some small nuance I need to have it call a specific tool, which then means the operator has to be very carefull to make sure only the tools I want to have used for that specific material in that specifc job are available to the machine. Groups helps some with this issue, but there still may be a case where I use a tool of a drill operation some of the time in a specifc material but want to use a different tool other times.
Bill Rutherford

North Woods Manufacturing

Full service CNC Machining

and Edge Banding

http://www.northwoodsmanufacturing.com

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Control Nesting tooling

Postby Brad McIntosh » Tue, Aug 15 2006, 7:47AM

Bill,

I see your point.

Perhaps a \"hybred\" could be worked out. Something that would specify the \"theoretical\" tool diameter and a TOOL-NAME to match for.

This way the genreral aim of the \"not-too-specific\" layer names is not lost but IF a tool that matches BOTH the \"theoretical\" tool diameter AND the SPECIFC TOOL-NAME (defined as the description? and not the tool number) as defined in Tool Manager, then that *special* tool will be chosen for that operation.

If a specified \"TOOL-NAME\" is not found in the description of a tool in the tool table, what should happen? Just go with the diameter match or throw an error?? (Perhaps that could be selected in the Control Nesting Settings at the machine.)

Sweet...

User avatar
Bill Rutherford
eCabinets Beta Tester
Posts: 386
Joined: Tue, May 10 2005, 5:23AM
Location: Lancaster, NH
Contact:

Postby Bill Rutherford » Tue, Aug 15 2006, 8:02AM

Brad,
The only problem I see with tool name instead of tool diameter is the fact that the name would have to match exactly. IE.

3-8 mortise compression
3/8 mortise compression
.375 mortise compression
3/8\" mortise compression

and so on. Given that it tends to eliminate some of the generic nature of the tool names. What brought that part to mind is all the custom machining we do. You would be amazed how many ways there are to say 3/4\" Pre-Finished Maple PLywood :lol: :lol:
Bill Rutherford

North Woods Manufacturing

Full service CNC Machining

and Edge Banding

http://www.northwoodsmanufacturing.com

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Tools...

Postby Brad McIntosh » Tue, Aug 15 2006, 8:15AM

Bill,

Then that is where the specification should then allow someone like yourself to go ahead and specify a tool number.

They should then only put those instructions in very fine print at the end of the manual. ;) That way people that do not need the \"TOOL NUMBER\" thing can avoid problems and just let the regular automatic tool selection processes run.

(** But I still like my first two ideas!! :) )

User avatar
DanEpps
Wizard Member
Posts: 5852
Joined: Thu, Jul 28 2005, 10:18AM
Company Name: Dan Epps
Country: UNITED STATES
Location: Rocky Face GA

Postby DanEpps » Tue, Aug 15 2006, 8:20AM

Brad

Is this an area that could be enhanced by the use of AFL to prompt for the \"spec\" and \"actual\" tool sizes?

User avatar
Bill Rutherford
eCabinets Beta Tester
Posts: 386
Joined: Tue, May 10 2005, 5:23AM
Location: Lancaster, NH
Contact:

Postby Bill Rutherford » Tue, Aug 15 2006, 8:23AM

Brad,
That completely cool with me. Heck, it might even make me feel special :oops:
Bill Rutherford

North Woods Manufacturing

Full service CNC Machining

and Edge Banding

http://www.northwoodsmanufacturing.com

David Hall
eCabinets Beta Tester
Posts: 588
Joined: Tue, May 17 2005, 12:41PM
Location: Stamford, CT USA
Contact:

Postby David Hall » Tue, Aug 15 2006, 10:59AM

There are some great ideas here. I too would find it useful if we could avoid reprogramming because of a tool diameter change.

Some time ago I requested that the chain compout and chain compin commands default to the outline tool if no tool diameter was specified. This would take care of some instances of the problem and I hope that it's still on someone's list.

I'm wondering if we already have a tool (no pun intended) available to us for this problem.

What does \"Substitue Tool Number\" in tool set-up do? I can't find any explanation in the super-control manual but seem to remember that if a tool's \"Life Left\" reached 0 then the subsitute tool (if specified) would be used instead. If indeed it does work this way then we might, maybe, possibly, could:

Set-up a tool (#1) with the programmed diameter, it's \"life left\" set to 0, and a substitute tool number of 101.
Set-up tool #101 with the actual tool diameter and no substitue tool number.
Hopefully CN would find tool 1 and use it without complaining. But when the actual tool change happens, tool 101 gets called and it's radius compensation gets applied.

If anyone get's a chance to test this... I'd love to hear the results. Be sure to measure daylight values for both tool 1 and 101.

Regards,
Dave
David Hall
Hall's Edge Inc.
eCabinets Machining Services
http://www.HallsEdge.com

David Hall
eCabinets Beta Tester
Posts: 588
Joined: Tue, May 17 2005, 12:41PM
Location: Stamford, CT USA
Contact:

Postby David Hall » Tue, Aug 15 2006, 12:04PM

Update.

It works!

But not for pockets. Pockets are essentially translated into a series of centerline operations by CN, using the diameter of the tool as programmed. Although the expired tool is replaced by the substitue tool, because there is no radius compensation used when cutting a pocket, the resulting pocket is the wrong size.

But for chain compout (and I assume chain compin, when it works at all) it works.

Regards,
Dave
David Hall

Hall's Edge Inc.

eCabinets Machining Services

http://www.HallsEdge.com

User avatar
Brad McIntosh
Guru Member
Posts: 480
Joined: Wed, May 18 2005, 6:59PM
Company Name: CNC Automation
Location: St. Zotique, Québec, Canada
Contact:

Subsitiue Tools

Postby Brad McIntosh » Wed, Aug 16 2006, 1:31PM

David,

The SUBSTITUE TOOL number was intended for those who were doing LONG production runs. In these situations, many times a tool may become dull and begin to effect/affect (??) the cut quality. If the average tool life in hours is determined and entered in to the Tool Table - then a SUBSTITUE \"SHARP\" tool can be specified in the box at the upper right.

If the LIFE LEFT counter runs out, the machine will continue to complete the current set of operations with that tool. Once a tool call is again made to the initial tool, the control sees that it has EXPIRED and will redirect to the SUBSTITUE, if present. During the substitution, all tool parameters and tool change locations assigned in Tool Manager to the substitue tool will be used (Diameter, Daylight, Tool Change Position, etc...).

Result: The long production run can continue uninterrupted! :)

I believe this feature was introduced for large, big production run companies that had Bulk Tool Changers, etc... But there may be an application for this feature for others not running hundreds and hundreds of parts in one run.

Hope this helps... :)


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: Bing [Bot] and 4 guests