Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: cjmerlin on July 13, 2012, 11:11:33 AM
-
Hi all, I've been recently trying to get to grips with threading on my Denford Orac machine it's not something I've done alot of on the cnc.
The problem I am having is that the thread is not cutting deep enough on an internal thread for the values I am entering into the threading wizard v1.17.
I have adjusted the backlash to zero in software (only 0.035mm in Z and oh my 0.09 in X)
I have adjusted the v point tool offsets (Glanz internal insert tool) so the point just touches the internal bore at 44.67mm
I require a thread pitch of 1.25mm and my math works the depth out using pitch * 0.866025 for crest to crest thread.
So in the wizard X start of 44.67. and the X end value of 45.7525. First pass depth of 0.15 which works out at 20 passes.
The lathe is started and threading commences, all sounds good and small swarfs of aluminium on each pass.
Removed billet and inspect thread, thread is cleanly cut, tracked perfect but the internal crest has a flat of approx 0.5-0.8mm on it.
I've done this thread several times and they all come out the same.
Is my maths wrong or is there something I have overlooked in software settings.
I know I can bodge the figures to "get in right" but I will be doing a large amount of threads at differing diameters so I am trying get the sums right first.
Any advice helpful.
-
When I was altering the post processor for Dolphin I messed about with the numbers and got it to do the calcs for me and with your start of 44.67 I would have an end depth of 46.17625
Looking in my PP what I have is for end Dia is (start Dia + (pitch x 1.205))
It seems to work well for me as I very rarely have to run a second, altered depth, pass on either external or internal threads. For external I have (Start Dia - (pitch x 1.32))
Hood
-
Hi Hood, Thanks for that info, I'll give that a try tomorrow, I had a go at doing an external thread as it is easier to check with the thread gauge, same problem so I adjusted the code to cut deeper (start dia - pitch) and although it was deeper there was still a flat on the crests so it looks like your numbers should get me there.
Had loads of fun with it today, no work done but still loads of swarf on the floor. ;D
-
Ha ha yes I still like seeing it do threading even after many hundreds of times. Probably because I have done so many manual threads over the years and just marvel at how simple it is on the CNC. I often do parts on the manual lathes if they are simple but if they need a thread it will be popped into the CNC for the threading, just so quick and easy :).
Hood
-
BTW there should be a crest on the thread but if you have a full profile tip it will be that that forms it.
Hood
-
Here is a close up of a M16 ( 2mm pitch) thread on the pullstuds I made for the mill, its hard to take pics of threads as the camera seems to bend things a bit, or does for me ;) but you can see the crest on the thread.
Hood
-
Nice threads there, i'd be chuffed at getting those. My insert is just a v pointed tip so when I get to the crested form I can adjust back a bit until i'm happy with them. Most of my threads are going to be quite fine pitch (0.5mm) so my accuracy is needing to be spot on.
John
-
FWIW,
The finer the pitch....all the more important on the set up and even a little backlash such that it screws up the depth of cuts can
end up with a bad thread. Have fun threading,
RICH
-
Yay I've got threads. I tried your info on the external thread and got a nice finished thread with a well defined crest.
I then then tried a 0.5mm external and that was good as well.
I then turned to trying an inside thread but still had a good flat on the id so I need to investigate why that happened.
All in all not a bad day.
-
Just have to increase the 1.205 multiplier a bit until it works out right for your lathe I suppose. Why it doesnt work for you and does for me I am not sure, could be backlash I suppose.
Hood
-
Hood, I think it would depend on the tool tip radius. John's probably sharper (smaller radius) than yours.
Dan
-
Hi, I did a few internal threads today and found that I needed to adjust the value to pitch * 1.3 to get proper crest form.
The insert tip even with my magnifier looks to have no radius (or perhaps so small I cant see) I also checked to see if it really was a 60 degee tip. I've checked tool offset and backlash, all good.
Still I suppose when it comes down to it, if it works don't worry about it.
John
-
Could well be that it is a sharp point. I use full profile tips so going from pitch to pitch the number I use will likely work out because of that.
Hood
-
Hi John,
The number you arrived at seems to be right based on the mathematical formula for a 60°: DOC = 0.5 x Pitch x tan60° ≈ 0.866 x Pitch ≈ 1.3
Dan
-
Thanks guys for the help and reassurance. I've now added a few buttons on the threading wizard to automatically fill in the X end value for the thread based on the formulas.
ATB
John