Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

mill/turn center drilling

tomwalls

New member
The knowledge base lists a technique for drilling a side hole ina part with a mill/turn center, and it works just fine as far as making it play on the screen. However, since the coordinate system is rotated from the one used for turning, the post thinks an axis has indexed, such as an A or B axis on a mill. This is not what I want. So, is there a way around this? Or, as I fear, will I have to create some custom post commands (I use Pro/NC Post), use some GOTO points instead of an actual holemaking sequence? I'm versed enough in Pro/NC Post to do this, but it seems to me there should be an easier way...


Thanks in advance.
 
Good Morning sim man,


It has been a while since I have worked with a mill turn center but I would try this. Create a different coordinate system that would apply the proper coordinates to the output. Use this as the output csys to the cl file in the sequence and post the results. I am not sure if this will work but I would give it a shot.


Also, if my memory serves me right, this should be a "point to point" output correct? If it is, thenthe Pro/NC sequence should be defined as a five axis drilling toolpath (there may even be a parameter you can change to fix your problem). Or isthe machine capable of reading a drill cycle in a multi-axis position and this is the approach you are taking?


Anyway, I hope this helps! Good luck!
smiley24.gif



Christopher
 
I have solved this by, Yes, adding 2 more sections in my FIL file. When you are coming from the side, you are actually rotating an axis that the lathe post cannot understand properly. Proe outputs the code in MULTAX data. You have to trap this in your FIL file in 3 places, "CIMFIL/ON,GOTO" AND "CIMFIL/ON,CYCLE", and "CIMFIL/ON,MODE".


In both macros, you will need to see if it is in "MILL" mode and then get the number of arguments in the CL record, when in Multax mode, the number arguments is 11. Then adjust the code so that you get the proper "X" and "Z" values.


This will be a tedious task to get the code exactly like you want it, but in the long run, it saves a lot of time. You will find out that you see on the screen is exactly what the machine will do.
 
Sim Man,


Pro/NC outputsSPINDL / PARLEL, XAXIS to indicate that you are doing side operation. Key in on this for tool orientation.
 

Sponsor

Articles From 3DCAD World

Back
Top