Problem with compensation offset in Siemens Mill-Turn PP and drilling

[apsTWRDF]

Hi guys,

I have two problems at the moment:

1.  I just got my double tool holder which allows me to mount two drills  in one tool slot with an X-Offset. So I added two tools with the same tool number and for one the necessary compensation offset of 50mm. 

Tool 6/A is a spot drill and Tool 6/B is the actual drill. When I start the program Tool 6/A spot drills perfectly and when the program should move on to the drill it doesnt seem to take the offset and its using 6/A. 

again as visible in the Gcode. 

2. For the spot drill it uses the spindle to drill (SETMS(1) at N22. But for tool 6/B it generates a SETMS(2) even that its not set as live tool in the  tools settings under Postprocessor.

Guess that needs to be modified in the PP somehow?

Would appreciate if someone could guide me through that.

Thanks,

Jochen

[da_fish]

I tried to reproduce your issue based on the description you gave and post processed it with your post but it work as expected for me. It could be something wrong in the Fusion file. If you could share your file I would be happy to take a look.

[apsTWRDF]

Hi,

thanks for your help. I finally found the problem with the SETMS(1) command. Tool was linked to the old tool Library where I used it as live tool. Stupid mistake.

To my second problem:

I think the diameter offset is the wrong way to do it.

Any ideas how I can shift X for 50mm to work with the second tool in that holder?

Do I need to add a second cutting edge like T6 D1 / T6 D2 and set the zero of each on my machine  (Sinumerik 828D) to get the necessary offset for D2?

Thanks,

Jochen

[da_fish]

I'm not familiar with siemens programing but I am familiar with running dual station blocks on Turn/Mills. I think your last statement is correct. Each tool should have it's own offset number. The Diameter offset in fusion is to specify which offset number to read from on the machine, Not the amount you want the tool to be offset. In my case, for the first tool I would use the offset for that station (tool 6, offset 6) and then for the second tool I would use a free offset like 13.

With a little bit of digging, it seems like siemens handle tool offsets quite differently than the DMG Mori machines that I'm used to. So you might need to take what I said with a grain of salt. 

Please let me know if that is or isn't helpful.

[da_fish]

Tool 6 and 13 (or which ever offsets you use) should than have different X values based on the spacing of the tools in the block.

[apsTWRDF]

Yes, just added an additional cutting edge to tool 6. Standard is T6 D1 for Tool 6 and Edge 1. I added another edge D2 . Now I was able to measure the second tool in that block in X and Z. 

So far so good... now I just need Fusion to produce the correct D value output for each tool in the code. At the moment both run under T6 D1 

Edit:     

A first test run where I manually edited the code to T6 D2 for the second tool worked perfectly.

[da_fish]

The question then is how do you want to define that. If you change your post processor so that the D value would reflect the offset value in Fusion, that could be a problem, since by default that number is equal to the tool number and all the previous programs you wrote would have to be changed or the wronged offset would be called.  

One suggestion, you could define it with the "Turret". Unless you're running a multi turret machine.

[apsTWRDF]

Thanks, that would be possible. Never worked with that option....  I have to have a closer look at that!