Siemens Turning Post issues

[tony3W49B]

Hi,

Can anyone help with this, please. I have a XYZ Lathe with with mill/turn capabilities with a Siemens 828D control.

I am using the Siemens generic turning post, and with my limited capabilities have managed to make some tweeks (M code for coolant parts catcher etc). However, when posting out programs I have come up against a couple of issue, listed below:-

1.For drilling cycles, the feed rate is posting out in a figure of mm/min, but the the control is taking this as mm/rev. F150. is being taken as 150mm/rev, for me the feed rate should post out as say F0.2.

2. Again, in the drilling cycles, the canned cycle is containing a G18 rather than G17. I am having to go into the cycle, in the machine, and manually change this. This is causing the machine to move 5mm in the Y+ direction and not move in the Z- direction. 

3.At the start of the programs a G18 is being posted there also.

I have checked the set up orientation, within Fusion and this is correct.

EDIT***** the drills I am using are in the turret and not in driven tool holders, as they are drilling on centre line******

Any help on this,  would be greatly appreciated. Maybe I'm using the wrong Siemens post contained within the library, or maybe someone has a working 828D Mill/Turn post that they are willing to share.

Once again, thanks in advance.

[christopher.cooperVHK2N · Accepted solution]

@tony3W49B Is the drill marked as a Live tool in the Post Processor tab?

Depending on the post used this could see the drill as a rotating tool and result in Feed per Min and not Rev.

[tony3W49B]

Hi Christopher,

I will check the process , but I’m pretty sure the drill was described as a non live tool. Thanks for your advice.

[serge.quiblier]

Hello @tony3W49B 

1 - Fusion is actually only outputting feedrate as unit per minute for the drilling for milling AND turning operations.
There is some work in progress to enable the user to select the feedrate unit mode. (no launch date defined actually)
2 - This is the plane selection command, it may be needed for drilling radially, or on the face (face is the XY plane so G17, radial drilling is XZ or YZ, G18 or G19 respectively). If you are sure, the machine does not need this, it can be removed from the onCycle function, it's the code
writeBlock(gPlaneModal.format(getPlane()));
3 - Same solution, search the onOpen function, and i suppose there is a line:
writeBlock(getCode("FEED_MODE_UNIT_MIN"), gPlaneModal.format(18));
change it to
writeBlock(getCode("FEED_MODE_UNIT_MIN"));

Cheers

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[tony3W49B]

Hi @christopher.cooperVHK2N ,

This was indeed the problem. The tool was selected as a live tool.

Thank you for your input, very much appreciated.