Well said Gary.
(even though long winded)
John,
That cabinet was cut out will a 1/4" bit.
I drilled with a 5mm bit.
Well said Gary.
(even though long winded)
John,
That cabinet was cut out will a 1/4" bit.
I drilled with a 5mm bit.
Same here.. I messed with it a bit. But Im in the middle of a large commercial job and I couldn't change mid swing.
Ok, thanks Gary, I see the issues. I guess this is the same thing Ryan P. was telling me but I didn't get it. I do have an addition to CPP to do a manual tool change; I haven't tried it though. Adding the air drill is probably the best bet, but I can't afford that just yet.
Roger, what kind of 1/4" bit are we talking about? One that can cut cabinets well without too much deflection and can drill peg holes without burning the veneer ply. Also, what feed rates are you cutting? The good part would be a little better yield...
The bit I am using for this testing is a 1/4" 2 flute compression bit. Solid carbide. I generally cut cabinets with a 3/8" bit. But I have designed this test cabinet around a 1/4" bit.
If you are going to use 1 bit for drilling and cutting I would think a straight cut bit would be the way to go.
I have an PRT Alpha with a 3HP spindle. I am cutting at 12,000RPM and at 6IPS with this 1/4" bit.
I cut at 8IPS with a 3/8" bit.
Both at 2 passes.
The neat thing about this software is that it is smart enough to cut full speed for larger parts and slow down for smaller parts. So ideally you can cut as fast as your machine/spindle can handle without thinking/worrying about the parts moving around.
Something else I like about this software setup is that on 2 passes for cutout it cuts the first pass on all parts then goes back and completes the cutout on the second pass.
So the first pass could be 12IPS and the second could be at 2IPS for parts smaller than 100^2 and at 12IPS for everything else.
I have said it before.
It is so nice to have this kind of intelligence available to us on our machine.
Where do I find the content for the C6, C7 and C9 files to enable the Link to call up different tools? For control software, I'm running version 3.6.1 beta 32, and am only finding generic text in these files.
Nat...
Until SB releases an official version of these toolchange files, if send me your my_variables file, and a copy of the new segment postP section for each of your drills, and I can build a version for you that should work.
Gary
Thanks Gary, I just sent the info.
Nat
I have recently upgraded my processor to handle small parts better. It seemed that smaller parts seem to move at the end of the cut through pass. I modded my software to place a 1/4 tab about 1" from the end, then go back and cut the tab very slowly. This seems to get rid of the little "ski jump" at the end. I can now cut 3" X 12" toe kicks with no problems. I am back on my fuji pump with 7" total vac.
I cut only melamine.
My question is, can something like this be put into the shopbot link?
Bob...
This feature and many more like it are already in there.
You have the option to define the area or width (or both) of small parts and then use a combination of: 1)Tabs, 2)Reduced cutting speed, 3)Leave user defined onion skin on.
Once you set this, and assuming you do not uncheck these options, future jobs will cut using these parameters. You can of course turn them off or change sizes and speeds.
The only feature that I personally find lacking is the ability to do profile cutting in the climb/conventional 2 pass onion skin method. The ability to do this has allowed us to increase cutting speeds close to 50% (to6 & 8 ips from 4ips) on our machine over a typical 2 pass method.
This has been put on my "wish list" and forwarded to the SB Link development team at Thermwood. If you use this method and are interested in or using the SB Link, voice your vote here and I will post a link to this thread on the eCabs Beta Forum. (which most cant see)
Gary
Strong vote here for the climb/conventional option.
With 1/4" back dadoes, and just the one cutting head, I'm confined to doing my perimeter cuts with this same 1/4" bit.
This bit size coupled with the tolerance of my machine, gives me significant deflection, even at 4ips. The cut/climb method is the only way that I've found to combat this, while at the same time producing decent edges on my parts.