male dovetail tool snapping

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

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

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

male dovetail tool snapping

Postby Mark Hesketh » Wed, Nov 21 2007, 11:32AM

I am having trouble with cutting some dovetail drawers today. I have just replaced the 1/4 dia downshear bit which is used for the male dovetails for the 5th time over 5 sheets of drawer parts. The bit keeps snapping right at the collet. I even replaced the collet after the second one snapped, there is no visible damage on the new one.
I have the spindle speed set to 20000, feed rate 400, dovetail feed rate at 100, plunge rate at 75, and I have made sure that the flutes are not set within the collet.
I am down to my second last bit and still have 3 sheets of drawers to cut... any ideas as to what I can do to avoid having my bits snap?

Ryan Hochgesang

Postby Ryan Hochgesang » Wed, Nov 21 2007, 12:03PM

Hi Mark,

First thing I'd suggest in this situation is to slow the Feed speed a little bit, maybe to 300 IPM. The other thing you may want to look into would be the SETTINGS, Blind Dove Tail button, Material Thickness to run outline cut value. This will help reduce load on 1/4\" cutter if you are not already using this feature.

Hope this helps!

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

Postby Forrest Chapman » Wed, Nov 21 2007, 12:25PM

Mark,

In order of cuts is it cutting the tails down to thickness first? I use a 3/8 downshear for this. This removes some of the material and tension on the bit. I prefer not doing the outline cuts around the tails as this nearly doubles the time cutting a sheet.

My cutting speeds for 5/8 baltic birch plywood are 600ipm at 18000rpm and 400ipm plunge with a 1/4 compression bit. Since Thermwood changed the order of cuts I haven't broken any bits.

I would suggest buying a bit with a short cutting edge no more than 1\".

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 » Wed, Nov 21 2007, 12:36PM

Ryan
As soon as it picks up the 1/4 bit, we are cranking the feed override down to about 50%. I just set the material thickness setting and am waiting for the code to write to try again (btw, it just snapped another bit... now I am on my last one) I will let you know how it goes.

Forest
It is cutting the tails down to thickness first, but it also uses the 1/4 bit for that... how would I get it to use the 3/8 bit? I was also thinking about the smaller cutting length, and am just waiting for a call-back from our local tooling guy to see if he can fed-ex me a few.

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 » Wed, Nov 21 2007, 12:38PM

Forrest
I appologize for constantly spelling your name wrong. I thought about it about 2 seconds after I hit the submit button.

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 » Wed, Nov 21 2007, 3:21PM

ok, set the material thickness setting so that it would use my 1/2\" outline tool to hog out around the tails... only problem is that the outline tool cut too far. It took off the tips of the tails, and made nicks in the body of the drawer box part. I checked my diameters and they are right. I also tried changing the spindle speed to 18000, and slowed the feed rate to 300, with a dovetail feed rate of 75. No matter which setting I tried, I still broke bits.

I don't understand why I am suddenly having this problem... and it isn't even a friday! I cut dovetail drawers at least once a week, and it has never been like this. I just spent 8 hours cutting out drawers that should have been done in about half that time (and lost 6 brand new bits in the process).

I have just ordered some 1/4\" bits with a 7/8\" cutting length, see if that helps. Should I be getting some straight bits, or remain with the downshear? or is there anything else I should be changing? I just don't want to run into this problem again. :wall:

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

Postby Forrest Chapman » Wed, Nov 21 2007, 3:58PM

Mark,

I think one problem is the downshear. This type tool cannot cool as quickly as an upshear or comp. type bit that removes material and heat while it cuts. The heat will rapidly dull the tool putting more pressure until it breaks.
I have 4 tools setup for drawers. The outline tool is a 3/8 comp. bit. Then a 3/8 downshear for dados and a 1/4 comp. for tails and a bottom groove and of course the dovetail bit.
My router takes the 3/8 DS and cut the tails to thickness. 2nd it takes the 1/4 comp. and cuts the bottom groove and then the tail outline. 3rd it outline skins the parts with the 3/8 comp. 4th it cuts the dovetail sockets. And then it final outlines.
This has worked well for me.

Forrest

Ryan Hochgesang

Postby Ryan Hochgesang » Wed, Nov 21 2007, 4:06PM

The down shear is likely creating a load of chips right at the tip of the tool causing additional pressure on the cutter in this case. Would be my last choice of cutter. As Forrest has mentioned I would use the compression or an upshear. However, the upshear may cause you to pull up parts if your vacuum is not sufficient or possible chip edges of material depending what your cutting.

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 » Thu, Nov 22 2007, 8:25AM

alright. Thanks guys. I will place an order for a couple of 1/4 compression bits.
Forrest, how are you forcing the machine to pick your 3/8 bit for cutting the tails to thickness? My machine only will if it is one that has been sharpened a couple of times and has a smaller diameter, otherwise it always picks the 1/4 bit... which is probably weakening the bit alot since the entire load would be on the last 1/4\" of the bit.

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, 10:18PM

Mark,

I guess it matters what thickness material you are cutting. In my case thats 5/8\" with a tool for 5/8\". This means your tails will be a little longer than 3/8\" and require a larger diameter bit. It also needs to be aranged in order before the 1/4\" tool.

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, 7:12AM

ah yes, I keep forgetting about the order of the tools. Don't have any time for the next week at least to play with drawers, but I will have to give that a shot when I get the chance.

Thanks again Forrest and Ryan

User avatar
Brian Shannon
eCabinets Beta Tester
Posts: 979
Joined: Thu, May 19 2005, 10:50PM
Location: Los Alamos, CA

Postby Brian Shannon » Fri, Nov 23 2007, 12:28PM

Mark,

Make sure your outline tool is the 3/8\" bit. Also, when I was cutting 12mm drawers with that setting, I received an error that said it cannot use a 3/8\" cutter for outlinearound male tenons. I had to change my dovetail width(eCab setting) to .5\", then RN would write proper code to use the 3/8\" for outline around tenons. Don't know if this is any help to you but it's worth a try.


Brian


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: No registered users and 7 guests