PDA

View Full Version : Inside square corner "over-cut?"



woodturner
01-12-2018, 07:08 PM
Hello all. Wondering if there is a setting I can modify for this. I've searched the archives to no avail. Trying to make an mdf Shaker style door. I used to get pretty clean corners with "Free Doors" before I got got into V Carve Pro. Using a 90 degree bevel bit and the inside profile with the square corner option. The tool "over-cuts" the corner in the M3 move. I've tried editing the bit setting from 80 degrees to 110. Under 90 gives straight a straight line segment over-cut corner. Over 90 and it starts to do a rounded over-cut. FYI, Alpha, spindle, 3mm per pass to 6mm deep, 8k rpm at 20mm/sec. Any thoughts are appreciated. Thanks.

steve_g
01-12-2018, 10:20 PM
I wonder if this will do what you need?
SG

srwtlc
01-13-2018, 12:07 AM
A picture of the issue would be helpful. Maybe even the problem vcp file.

steve_g
01-13-2018, 04:02 AM
Well… I thought maybe the allowance box was something magic… I took the time to learn what it was about and no, it’s not. I guess Scott’s suggestion for pictures or code is the next step to help us understand the problem better!
SG

woodturner
01-13-2018, 12:02 PM
Hi and thanks for the responses. Steve, that is the option I've been using for the inside square corner. I will take a few pics and post on Monday. Below is a test to 3mm deep (1 pass) and the bit (lie to software) at 89 degrees.

MS,14.9,14.9
JZ,8.000000
J2,200.000000,300.000000
J3,2006.500000,324.450012,6.000000
M3,2006.500000,324.450012,0.000000
M3,2009.448120,327.398102,-3.000014
M3,2009.448120,381.501892,-3.000014
M3,2006.500000,384.450012,0.000000
M3,2009.448120,381.501892,-3.000014
M3,2043.551880,381.501892,-3.000014
M3,2046.500000,384.450012,0.000000
M3,2043.551880,381.501892,-3.000014
M3,2043.551880,327.398102,-3.000014
M3,2046.500000,324.450012,0.000000
M3,2043.551880,327.398102,-3.000014
M3,2009.448120,327.398102,-3.000014
M3,2006.500000,324.450012,0.000000
J3,2006.500000,324.450012,6.000000
JZ,8.000000
J2,200.000000,300.000000


Thanks Again!

Brady Watson
01-13-2018, 12:53 PM
How's the preview look? Is this where you are seeing the overcut corners or at the machine?

Post the VCP file (after you WinZIP it) - otherwise, there isn't a whole lot we can do for you...

-B

woodturner
01-13-2018, 01:44 PM
Thanks Brady. I can't really see it in the preview. I have to zoom in to where it gets blurry. I see it in the test cuts. Pics on Monday will (hopefully) show it clearly.

woodturner
01-15-2018, 10:39 AM
Good Morning...http://www.talkshopbot.com/forum/attachment.php?attachmentid=31078&stc=1http://www.talkshopbot.com/forum/attachment.php?attachmentid=31079&stc=1

1st pic shows results of inside square corner using 95 degree included angle (rounded over-cut) on the left and 90 degree included angle (straight line over-cut). 2nd pic shows extremes, 80 degrees-top, 100 degrees-btm. 89 degrees used to work best with "Free Doors" and I started with that, but it was worse than 90.

This morning I tried another "work around." I had it profile cut (with 89 degree setting) inside the vector using inside square corner (actually listed as "Sharp internal corners 3D) to 3mm deep. Then I offset the vector (inward) by 4mm and re-cut 4mm deep WITHOUT inside square corners checked . The deeper pass sort of caught up to the over-cut and gave a much better result. What a pain it'll be to do every custom door this way but I don't know what else to try.

Again, any ideas are appreciated. Thanks,

srwtlc
01-15-2018, 10:58 AM
Are you sure about the angle of the bit? Is this the same bit that worked before? Has it been sharpened lately? Are you zeroing on the surface of the material or on the table? If on the table, do you have the exact thickness of your material set in VCP.

woodturner
01-15-2018, 11:48 AM
Hi. Pretty sure about the bit angle. Tucks in nicely to a machinists protractor set at 90. Not sharpened, carbide insert though, but unchanged since the last run with free doors pgm (dedicated bit for doors). And, yes, zeroing to the top of the material. Thanks.

srwtlc
01-15-2018, 12:02 PM
Insert....is the point dead center? Lower it to just scratch the material (make sure material is secure) and give it a spin. If it draws a point, good. If it draws a circle, bad. Remount the insert to get it to draw a tight point.

Brady Watson
01-15-2018, 12:06 PM
My advice would be to step back....let's make things simple before getting into the door design.

Make a 1/2" x 3" rectangle & V-carve it with that same bit, with it spec'd out at 90.0 degrees. Does it come out right at the machine? If no, alter the angle with 2 more rectangles @ 89 & 91 degrees. Which looks better?

-B

woodturner
01-15-2018, 02:02 PM
Hey guys. I checked the insert and it's almost a perfect point. There is a tiny dot of raised material dead center. Hard to get much resolution in mdf! I might try a new carbide insert and see if wear has anything to do with it. Also, I have been making small adjustments using a 50mm square and retrying the cut(s) with mixed results. http://www.talkshopbot.com/forum/attachment.php?attachmentid=31081&stc=1

woodturner
01-15-2018, 04:23 PM
Okay. My apologies fellas. Your collective posts got me to thinking. What possibly could have changed (beside the software) since the last time I tried this... Well, the Free Doors program required several tool changes using one spindle. With the new software, I had planned to take advantage of both spindles (and the air drill) for fewer tool changes. That's when it hit. I used to do the cuts with the "other" spindle. Tried with that one and it worked fine. Which, then led me to check set screws on the gear for the "A" vertical axis and there was some play. So, I'll have to set aside some time to pull it apart and "bend" some new allen wrenches. I'll use the "Z" to get through this job. I wish I could claim "newbie" mistake, but I can't. We just don't really use the bot very often and that's never happened before. So, in conclusion, sorry for wasting your time but thanks none the less. Kind Regards!

Brady Watson
01-15-2018, 05:46 PM
No worries - it happens!

If for nothing else, you posting this may prevent someone else from enduring misery & mystery - and give them another area to check.

It's been said a gajillion times - part of normal/regular machine operation is shaking down the tool in all directions, listening & feeling for play/slop.

PRTs are notoriously sloppy in the Z because the T-rails get worn causing it to come out of mesh with the pinion...PRSs get sloppy because the lower V-roller bearings are not adjusted properly, either because they were adjusted too tight from day 1 and roll forged the rail into the extrusion or just not bolted down tight enough.

-B