Heidenhain post customization

In this post you can find some notes on Heidenhain post customization.

Please send me an mail if you spot something wrong or not clear.

Here the current website to download the manual : https://content.heidenhain.de/doku/tnc_guide/html/

You can also download the programming station windows pc software to test the output gcode ( limited to 100 lines ) .

Here the link : https://www.heidenhain.com/service/downloads/software

The latest post processor is available from post processor download page.

Drilling macro

Additional explanation can be found also here .

The parameters requested from drilling macro.

The project example image , with indicated Z levels :

Here the parameters description :

Q200 : Incremental distance from Q203 . It's the z level where the feed change from rapid to work.

You set this value from post processor dialog > machined properties > safe approach distance in drilling cycles.

Q201 : It's the tool BOTTOM Z LEVEL . Incremental distance from Q203.

Q206 : Feedrate . Defined from tool cut data parameters

Q202 : Plunging depth step . Defined from tool cut data parameters

Q210 : Dwell time at top . Hardcoded value in post processor template.

Q203 : It's the START Z LEVEL absolute coordinate . See the drilling operation levels image.

Q204 : It's the SAFE Z LEVEL  incremental coordinate from Q203. It's the safe z level where the tool doesn't collide with anything.

Q211 : Dwell time at bottom expressed in SECOND . Hardcoded value in post processor template.

Here the [Deep Hole Drilling] template :

 CYCL DEF 200 DRILLING ~
 {NO_LINE_N} Q200={APPROACH_SAFE_DISTANCE} ;SET-UP CLEARANCE ~
 {NO_LINE_N}  Q201={INCRE_HOLE_DEPTH} ;DEPTH ~
 {NO_LINE_N}  Q206={FEED_VALUE} ;FEED RATE FOR PLUNGING ~
 {NO_LINE_N}  Q202={STEP_VALUE} ;INFEED DEPTH ~
 {NO_LINE_N}  Q210=0 ;DWELL AT TOP ~
 {NO_LINE_N}  Q203={START_Z_VALUE} ;SURFACE COORDINATE ~
 {NO_LINE_N}  Q204={SAFE_Z_INCR} ;2ND SET-UP CLEARANCE ~
 {NO_LINE_N}  Q211={DWELL_CODE} ;DWELL AT BOTTOM
 {POINT_LIST}

The graphic simulation from programming station :

Heidenhain programming station notes

To open the generated gcode press this button.

It will open the folder :

C:\Program Files (x86)\TNC320\771854\TNC\nc_prog

Save the gcode in that folder.

Press this button to start the simulation .

You can find additional simultation configuration scrolling the softkey indicated here .

In this menus it's available also the tool table .

By default the tool station is the same as tool radius.

Example . The tool at station 10 will have a tool radius of 10 mm .

You can edit the values in tool table. Press [END] when done.