I have a Bridgeport interact 1 series 2 fitted with a Heidenhain TNC150 controller. I now have a need to do a lot of contour surface milling which will exceed the controllers memory. To my dismay I discovered the TNC150 will not accept 'drip feed' data from an external source. I have looked about and found a Heidenhain TNC151A control which I am told can do the job - transfer lots of G code data from the output of my CAM program - Can anyone please confirm this to be true ? Any other info greatly appreciated.

Rgds


Dave

go to to the heidenhain website and get the tech manuals. I believe they should be plug ins, at least I was told by heidenhain that the 145-151 was, so I am assuming.

Very similar controls. But more parameters in the 151 (A and B). You will need a new parameter list.

George

I work with Dave - many thanks for the info - now have a new list and we think are getting there !!

One question though, with 'blockwise transfer' how do you set tool definitions ?? We keep getting the error 'Error Missing Tool Definition"

Many thanks Rob

my machine does not seem to care about that until it goes to run. Perhaps there is a parameter regarding use of a tool table or not, or other tool related parameter

perhaps parameter 225, if it uses it central tool memory, 0 or 1, opt for 0 perhaps

Many thanks Gus - Right on the button !! Parameter 225 was the one -
specified 20 and up came a tool table for 20 tools - magic !

Thanks

Dave

Thanks Gus,all is well with transfer of files and tool store.

might you have an answer to the following....when running our bridgeport both in blockwise transfer and files from control memory the table movement is very slow almost moving in step mode to each block of of program rather than a smooth flow and it's slowing the machining time down

Thanks

Rob

there may be a parameter that makes it stop at corners, or it could be that the accel ramp is overly conservative.

Now that yo are good at sending and receiving, make sure to store your parameters as they are, and you can play with a few things

parameter 91 is constant contouring on corners. As you approach 90 degrees you WILL get gross positioning errors. One of my machines I tolerate this and reprogram parts that I try to rapid this way, either by putting a .1 second dwell in between two moves, or changing the way it makes the move.

parameter 54 is the accel parameter You can play with it a bit, but make sure the machine is happy with what you choose. Bridgeport chose a pretty gentle
accel ramp, and you feel it on peck drilling. Over harsh and it will beat the machine. The weakness of bosch drives is probably this. The Copley drives I put in one of my retros allow a very steep accel ramp.

Get the control tech manual from the heidenhain website, it has a lot of good info

Thanks Gus,

All is good now,we have changed parameter 60 to 1 from 0 this has made a vast difference...the program run is smoother.....so we are well on the road now,so thanks again.

Rob