Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Siemens 828D alarms out and won't run F360 created g-code

andrewJ5JUW
Explorer

Siemens 828D alarms out and won't run F360 created g-code

andrewJ5JUW
Explorer
Explorer

Hi all.

I have a problem with G-code created in F360 not running on the Siemens 828D control fitted to my XYZ 750LR VMC.

I believe the error is to do with Tool numbering and have tried several changes / variations both in F360 tool library and in the tool library on the control to overcome it none of which have been successful.

The error code is:

17190 // Channel 1: Block N24 illegal T number 1

The line of code it flags on is:

N22 G0 SUPA Z0 D0

See screen shot called “error message in simulation.jpg” that shows the above.

If I quit out of simulation mode by pressing the // soft key and hit Cycle Start the code will start to run on the machine but then stops at the same place and alarms out.

This is my first CAM programme I am trying to run on the machine and I am new to F360 and quite new to Siemens / Shopmill also.

I am using the generic Sinumerik 840D post with no changes made to it.

I have attached some other images also that show my tool library in F360 and on the machine as well as some of the first few lines of code.

An help / suggestions would be greatly appreciated – right now I have learned enough to model parts and create tool paths in F360 and love the power of the tool am stuck to run even a facing op’ on a square block because of the issue above.

0 Likes
Reply
1,726 Views
5 Replies
Replies (5)

andrewJ5JUW
Explorer
Explorer

I have been reading lots and experimenting further on this issue and this afternoon had a break through.

 

In the "Post Properties" tab when post processing the job there are a couple of options I tried differently.

 

On the code that would not run I had the "Tool as name" ticked in preferences. I had the "Safe Retracts" set as SUPA - these are both settings that come when downloading the 840D post from the F360 post library.

 

I tried unticking "Tool as Name" and leaving Safe Retracts set as SUPA. The code still failed to run.

 

I then set "Tool as name" as ticked and changed Safe Retracts to "Clearance Height"

 

This version of the code ran on the 828D control in simulation. I then hit execute and cycle start with the feed rate turned all the way down and the programme ran OK. I let it go as far as changing the tool and starting to travel down towards the work piece and then Cycle stopped and came out of the code.

 

So I am glad I managed to get it running but now have a nagging concern that using "Clearance Height" instead of SUPA may have some as yet unknown impacts down stream.

 

The options for this setting are:

SUPA - (default setting for the as-downloaded 840D post from F360 post library) - this won;t run on the 828D

Clearance Height - this runs

G53 - I have not tried this.

 

If anyone reading this knows what these 3 different settings do and how they might change how the code runs then I'd love more information. Especially if there are some as yet un-known to me potential pitfalls for using one of other.

 

See images attached for the settings referred to.

 

0 Likes

jaredSADUH
Enthusiast
Enthusiast

I've run many machines with various controls, not so many with the Seimens control though.  My first thought was that the SUPA was confusing the control and Clearance Height should be selected.  Clearance height should have your tool go to the height you designate in your heights tab, or if outputting a G28 Z0. your machine should return to home, change tools (as needed/programmed) and continue running.  Some machine controls require the G53 instead of a G28, look up your make and model of controller to find the appropriate G codes.

 

When you say the machine did a tool change, moved downward towards part and then stopped and "came out of the code", what do you mean by that?  Was there an alarm that got thrown?  Was there anything in particular that happened besides the machine stopping?  Any message on the screen?

0 Likes

andrewJ5JUW
Explorer
Explorer

Thanks for your reply.

 

I was not very clear in my last reply. What I meant to say was that the g-code ran on the machine - meaning the programme started (rather than alarming out),  the spindle came up from where it was positioned and did a tool change, it selected the 80mm face mill (T1) - which is correct and as programmed , the spindle started and rapid down started - again as programmed.

 

I then purposely stopped the programme using "Cycle Stop" as my objective at that point was just to test whether the g-code would actually run lines without alarming out - I was not attempting to actually carry out the facing operation as the job was not even set up in the vice. It was Sunday and I was out of time.

 

Later this week I plan to actually set up a block in the vice and see if the code can perform the facing operation as intended. At this point all I know is the g-code with the different post processor settings actually runs where as when I logged  this thread I could not get it to run without alarming out. I don't yet know whether the cutter will go where it is supposed to.

 

I spoke with Siemens Tech support today and but no useful or actionable information was provided. I tried to get clarity whether changing the post setting from SUPA to "Retract Position" might have any un-desired effects but they could not tell me.

 

So I think cautiously testing the code on in a dry run with a large Z offset and reduced feed / speed is probably the way to go and see if it behaves as programmed / expected.

 

 

 

0 Likes

jaredSADUH
Enthusiast
Enthusiast
Hey, no problem. Like you said, cautiously run the program above the vise
and check that all movements are correct. You can scan your G code and
look at the Z numbers to check them out too, if you want to spend that kind
of time before the dry run. I always do a dry run when using a new post
processor just in case.

Good luck!
0 Likes

andrewJ5JUW
Explorer
Explorer

Just a further update on this issue.

 

I got some time between other jobs to dry run the G-code.

 

I am happy to say the code ran faultlessly end to end with no unexpected or spurious moves.

I then created some additional tool paths this time calling up multiple tools and performing facing, 2D profiling and 2D pocketing commands. Again - these dry ran 100mm or so above the bed without any issues.

 

So at this point although I have not actually cut metal with the code so I can't say if the tool paths are producing accurate results I am confident enough now to try machining some first test parts using F360 created code rather than code I have programmed on the mill using the Siemens ShopMill on the control.

 

This setting also allows Tool names to be as per the text in F360 e.g - 80mm face mill in F360 is fine and comes out as "T1" (80mm face mill). The tool name in the Tool List on the machine must match letter letter though. Easy enough to do. 

 

In summary - if you have an 828D control, and you use the F360 post that is published on their library for the 840D control (which is recommended by F360 when I raised the issue with them during a test drive before purchase) - don't leave the field for "Safe Retracts and Home Positioning" as "SUPA" - change it to "Clearance Height" and the code will run without alarming. Also - set the "Tool as name" check box as ticked so the control recognizes tool names correctly AND make sure the tool list on the machine matches exactly what the tool library name in F360 is - letter for letter.

 

Lastly proceed with caution - I have dry run this only.

0 Likes