male dovetail tool snapping
Moderators: Jason Susnjara, Larry Epplin, Clint Buechlein, Jim Bullis
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
male dovetail tool snapping
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?
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?
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!
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!
-
- eCabinets Beta Tester
- Posts: 1240
- Joined: Mon, May 30 2005, 2:26PM
- Location: Anderson SC.
- Contact:
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
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
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
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.
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.
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
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.
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.
-
- eCabinets Beta Tester
- Posts: 1240
- Joined: Mon, May 30 2005, 2:26PM
- Location: Anderson SC.
- Contact:
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
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
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.
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
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, 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.
-
- eCabinets Beta Tester
- Posts: 1240
- Joined: Mon, May 30 2005, 2:26PM
- Location: Anderson SC.
- Contact:
-
- Guru Member
- Posts: 366
- Joined: Fri, Aug 25 2006, 9:12AM
- Company Name: Paris Kitchens
- Country: CANADA
- Location: Paris, ontario
-
- eCabinets Beta Tester
- Posts: 979
- Joined: Thu, May 19 2005, 10:50PM
- Location: Los Alamos, CA
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
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