Results 1 to 18 of 18
07-09-2007, 10:06 AM #1
We just got a new Fryer ET30 with Fanuc controls. I'm trying to do a thread repair cycle with the help of the Manual Guide i and i'm having little success. Any help?
07-09-2007, 04:36 PM #2
What is a thread repair cycle?
Do you mean the Fanuc G76 threading cycle?
Tell us more.
07-09-2007, 05:26 PM #3
We build hydraulic cylinders. What we're doing is threading the ID of one end for the gland. I guess not every one was checked before it was removed from the lathe and now we have one were the gland doesn't thread in properly. Until now we've been using a manual lathe so this hasn't been a problem. What i would like to do, and according to the brochures on Fanuc's Manual Guide i this is supposed to be a breeze, is throw the tube back in the lathe, touch off on the bottom of one of the threads and program the TPI and the distance you want to go in and it'll take it from there.
07-09-2007, 05:56 PM #4
I am only guessing but I don't think your fryer has a servo spindle with encoder. That is a requirement for finding a thread sync point (as far as I know). You can still do what you want to with an AC spindle drive but it is a bit tricky. What you need to do is start your thread cycle like you normally would using manual guide but put a large enough negative wear offset on your tool so that it is clear of the thread during the cut cycle and adjust your thread cycle inputs so that the cycle makes only one pass. Once you do this, run the cycle paying attention to the alignment between the tool and the threads. Change the "Z" start point value in the manual guide cycle (Under Details) a positive amount that you think will get the tool and thread into close alignment (Alternatively, you can move your "Z" work offset if that seems simpler). Put some blue on the threads. Run the cycle repeatedly adding about .010" of positive wear comp each time until contact is made. Depending on which side of the tool makes contact first, and how much wear offset you have still available, you can calculate how much to change your final "Z" start point by. Make the change to the start point, remove all (or most) of your remaining wear comp and let her rip. Now isn't that simple? Aren't you asking yourself why that isn't in the manual? Call me at work if you want to go to the trouble of doing this and are nervous.
Glenn @ Metro North
07-09-2007, 06:59 PM #5
Thanks for that, it makes sense. I've been informed that this lathe has a Baldor AC spindle drive with an encoder on the spindle. Will this help?
07-09-2007, 08:34 PM #6
I think you are out of luck with the AC drive. I am only using mine as a reference though so more investigfation of your machine may prove me wrong. I think that the encoder feedback is only used to give a close spindle speed for threading as well as sending a "pulse" to start the threading feed. I don't imagine that you can rigid tap with yours either and if you could pick-up on and chase a thread then you could also rigid tap. Good luck with the chasing, Glenn.
07-10-2007, 08:16 AM #7
Could you send me a copy of the manual guide brochure page that mentions the thread chasing function? I have one lathe here with Manual Guide and an AC spindle and the other has Manual Guide and a servo spindle. The servo machine will rigid tap so I could test the function of the chasing on that machine if I could get some basic info about the procedure. If you could email me a scan of the page I will email you a scan of a toonie to pay for your time.
Glenn @ Metro North
07-10-2007, 11:04 AM #8
07-10-2007, 12:13 PM #9
I have a Romi with an AC spindle and it will index every 1* by program(M19 to oient then G64 C (angle). It will also rigid tap and orient the spindle (M19)
It has the thread repair and it works fine. (Fanuc 21i-T) There is a soft key selection in the setup of the thread repair to orient the spindle before you touch off the tool. You can modify the tool cut by using a shift of the start point. Can do single or multi lead threads.
Have never used it for ID work but the OD feature works fine....don't think an ID part would present any complication other than selecting "ID at the setup of the cycle.
07-10-2007, 12:55 PM #10
Don't know if the setup on the Romi is exactly the same as what you have but here is the brief setup info that i use:
Set the control to "jog" and "guide"
Key "cycle" to enter the cycle menu
Select "Thread" as the cycle choice.
Enter all the data as a normal ID thread ie: ID,Tool number, spindle speed,Spindle direction,Chamfer "OFF",Skip the cut amount for now, Type= General, and at the "Method" choice select "REPAIR".
At this point the Cut amount box will default to "Cut Times" and the number will be 1.0000. This can be changed to be back to "Cut Amount" and a value for the first cut taken by the tool, or left at "Cut Times" and you may use any number here for the number of passes you wish to make. The default is one pass because the intent is just to make a clean up pass, but you may use more if you wish or you may make a series of cuts to depth.
Finish by imput of the thread angle (60*) and the pitch or TPI and weather to use coolant or not.
Now you can orient the spindle. There should be two soft key choices on the spindle. One to "Orient" and one to "Cancel Orient" Select the "Orient" and the spindle should jog and stop. It will be held fast at the stopped position.
Yoy then need to enter your tool start and stop information. This can be done by entering the size and length of the part or by letting the tool measure the position. This is done by using the "RD POS" soft key. TRhis will enter the location of the tool into the program. I do not use this feature, but rather enter the start and stop points manually in the "X start" ,"Z start" and "X finish, Z finish" boxes.
If you used one cut in the choices above you will need to use the position of the tool at full depth as your "X" value. If you are using multi cuts from start then use the md as the "X" value...(try all this on some scrap before trying on the real part)
Now move the tool to a thread and position it as best you can in the groove. Hit the "SYNC P" key. This will now time the thread location waith the oriented spindle position.
Once the sync is done, use the "CAN Orient" key to reliese the spindle. Mover the tool clear or the part and cycle start....
Again try all this on an old part or in the air to see how all the commands relate. If you wish ot make a full thread cutting air for the part already done sue thje "Cut Amount" selection and choode the depth for your first pass. Spec the X start as the minor diameter and use the "detail" key to adjust the depth to give the thread depoth of cut you wish.
One further note: the cut timing can be adjusted by using the "shift Ofs" imput. Plus values here will move the tool to cut more on the rear of the thread profile, and a neg value here moves the tool to cut the lead side more.....Could also use this value to cut a multi lead i think but have not tried it.
07-10-2007, 01:07 PM #11
Mine does not have the same functions in it as yours. My guess is that it was left out of both my lathes by the builder when they spec'd the control options. My lathe with AC spindle will also not orient the spindle or rigid tap and also does not show the spindle orientation on the screen. I hope RedRon has the same functionality as you do.
07-10-2007, 03:05 PM #12
Yeah, i can't orient the spindle on that lathe but according to Larry Fryer of Fryer Machines i can rigid tap. i guess i'm SOL. by the way, i did try touching up the threads by grabbing the tube on the marks left from the first time i had it in the chuck, ran a wear offset on the X axis to just clear the threads and then adjusted the wear offset on the Z axis so that it lined up close to the center of the threads. Then i started taking a little off the X axis wear offset every pass and adjusting my Z axis as it needed. Only problem is that it started touching one side of the threads first, not serious but i figured it could be improved, so i hit Cycle Stop expecting that it would retract from the threads the return to the start point like it does on our Mori Seiki with Fanuc controls. I was wrong! it just returned to the start point from where it was at, dragging across the threads! No big deal though, cause we can cut that end off and shorten the tube up a bit and use it for one off our other models of cylinders. I just wanted to figure out how this works cause sooner or later i'll need to know.
07-10-2007, 03:28 PM #13
Your experiences, Alfa's and my own with three similar machines just show how differently the machine builder can make machines when they all use the same brain. On my lathe, cycle stop in the middle of a thread cycle only lifts the tool clear at the end of the pass. You can then restart the cycle where you left off as long as you don't leave the control mode that you are in. Have fun.
07-10-2007, 04:02 PM #14
i tried what you suggested as far as entering the program for the thread repair but i don't even have the 'Method' option under 'Thread Type'. i guess it would be useless anyway if i can't orient the spindle, eh? i guess it's just another feature on this machine that we were told it had but doesn't.
07-10-2007, 10:33 PM #15
This is what we were able to do to repair quite a few undersize threads;
Thread a new setup part and before you take it out of the chuck, spin a thread gage(homemade undersize just like the bad parts) into the part and then mark the gage and the chuck with a scrib line. Then when you rerun the undersized parts thread the gage into the part and line the thread gage scribbed line with the scribed line on the chuck. Then clamp the chuck and remove the thread gage.
hope that makes sense.
07-11-2007, 11:40 AM #16
That totally makes sense and is actually quite an ingenious idea! If this ever happens again, i'll try that. Only one problem though, what do you do if there's a repair project, something you've never made before? As far as for our production, i'm gonna get the guys to check all the parts BEFORE they take them out of the lathe.
07-11-2007, 12:29 PM #17
We do thread repair on oilfield tubing. Since we don't have a contolled spindle axis we have to go the long way around.
First thread a sample piece, using a set of dial calipers measure from the face of one of the chuck jaws ( I use #1 jaw all the time so I don't get mixed up), let's call this piece "fixed number". Next, put in piece to be repaired, dial in then measure from jaw face to thread root. Do the math, take the number from the piece to be repaired then subtract "fixed number". This give you the offset in Z axis. Move machine, run thread. Remember that you can reduce this number to the nearest thread lead.
It does take some practice but works well for us.
09-08-2007, 11:59 PM #18
Although this dosen't help your problem, what we do is mark a chuck jaw with a fine line and mark the part with a fine line. Place the part in the chuck jaws with these lines matching up. We then cycle the part(threading included).Remove part and check threads, etc., while next part is being machined.If the threads won't gage just place part back in jaws again with the aforemetioned lines matching up, re-run thread pass with proper adjustments made(offsets/new insert corner etc.).
This way you can gage each thread outside of the machine, keep the machine running, and be able to re-run parts during the same production run.