Machsupport Forum
Third party software and hardware support forums. => SmoothStepper USB => Topic started by: woffler on June 02, 2013, 08:25:47 PM
-
Hi everyone ,i am trying to research the encoder function of the ESS for spindle sync of my lathe spindle , i want to use the C53 board from CNC4 PC . http://www.cnc4pc.com/Store/osc/product_info.php?products_id=483
What i am wanting to know is has anyone done this and how did it work for them ?
-
You just need the index pulse on an input for threading on the SS or ESS, the axis is not properly synchronised to the spindle encoder unless things have changed very recently.
Hood
-
Thank's Hood i did get a hold of Greg i think that was his name ,from Warp 9 and he said he will be working on this and hopes to add the A and B channel's, sure would be nice.
I sure do not want to spend a couple thou. on a re-due ,seem's i am doing a lot of single pointing lately , a lot of wind mill banyan pump connecting shaft's of stainless steel for ranch's .
Lot's of water being pumped this time of year in Arizona ,and it is only 106 in the shade!!! :D
-
Yea they've been working on that A B thing for a few years now. I wouldn't hold my breath.
Derek
-
Woffler,
I do a lot of threading and the SS and ESS have always done nice threads for me using the index only form an encoder, are you having problems with it?
Hood
-
No, I have gotten it to work ,but I am getting a weird move out of Mach on the beginning of a thread file for a tapered thread .
It will make a rapid move to ( X0 ) from the offset position of ( X.84 Z0 ) when it is not in the G code program ,thus causing me to have to offset the (Z zero) by the with of the threading tool.
And as you know this affects the length of your taper and thread's per inch, is there a setting in Mach that could cause it to make this move?
I am going to attach the G code file so you can see it ,this happens before the spindle start, immediately from cycle start.
Thank's Woffler
-
What have you got set in General Config for the toolchange option? If its Stop Spindle then wait for start it could be something in the M6end macro, for Turn there should be nothing in it.
Hood
-
I have stop and wait for cycle start in general Config., i wrote another program for 2 inch pipe and got the same result it just want's to dive right in there to X0.
It must be in the Macro ,I would not even know how to look at it and find and correct it. ???
-
In Mach go to Operator menu then down to VB Script Editor.
The Editor will open then go to File menu then Open. Browse to the macro folder of the profile you are using and double click M6End.m1s.
It should have
REM nothing here in lathe
in it, if it has anything else delete it and paste in the above, click file and then save and then close the editor and see if your issue is still there.
Hood
-
I found a lot in there ,am I supposed to delete everything? I attached the file so you can see it.
-
Yes delete all that crap, that is the standard M6End for a mill profile. I think at some point you mus have either just used a mill profile and changed it to a lathe profile by changing the screenset file extension, or possibly you cloned a mill profile to make your lathe profile.
Hood
-
That fixed it , I must have borrowed the lathe profile for my A axis on my mill when I run it with A axis spindle and do some turning on the mill. ::)
My bad ,it usually is me that screw's things up ,I just converted the lathe to CNC a little while ago and I am still getting use to it .
I am finding that I should have done this years ago what a time saver ,I still have trouble getting use to how accurate it is ,this is the first hiccup I have really run into.
I am so use to sneaking up to a dimension I can not get over it ! I am trying to modify my post's now and get that finished to eliminate some steps there as I see some unnecessary moves in the G code files ,I am trying to do this in between job's but it is going well .
Thank's for the help Hood
-
Thats good, and yes a CNC lathe is very nice, especially if its a complex part or has a thread on it.
I still use my manual lathes quite a lot, probably more than the CNC ones. That however is because of the nature of the things I do as often I am repairing parts that would be hard to get set up on a CNC lathe or at least is just as quick to do on a manual lathe.
Any threading however, even if I have done most of the rest on the manual, gets shoved in the CNC as its just so quick and easy to thread with CNC.
Hood
-
I am looking for another to make shafting on with a larger swing and threw hole ,but everyone i have looked at so far is worn out . Do you use a G76 threading cycle with Mach 3 if you do could you send a little snip-it of code for an example.
-
Yes I use G76, the simple threading wizard will produce good G76 code for you if you want to take a look at that.
Here is a G76 for an internal thread
G1 Z6.0 X38.0
G76 X39.808 Z-18.0 I29.0 P1.5 H0.4 Q03 T0 C1.0
G0Z6
And an external
G1 Z6.0 X60.0
G76 X58.02 Z-18.0 I29.0 P1.5 H0.2 Q01 T0 C2.0
G0Z20Hood