Router just raises and trips Z limit switch

[eisenmanguitars]

When I open this process up in UGS, and start the operation, my router raises up and hits the limit switch immediately.  I have no error notifications in my setup or toolpath.

I'm assuming it's a setting in my manufacture tab.  FYI I erased an old project off this file, incase anything weird is left over.  Any idea what I did wrong? Here's what UGS says:

>>> G90
>>> T1
>>> S5000M3
>>> G54
ok
ok
[Error] An error was detected while sending 'S5000M3': (ALARM:1) Hard limit has been triggered. Machine position is likely lost due to sudden halt. Re-homing is highly recommended. Streaming has been paused.
[MSG:Reset to continue]

[GeorgeRoberts]

Good morning

A few questions regarding this: 

• Does your machine move at all? It should home in Z prior to the codes you shared in the message
• Do you have a programmable spindle and can it go to 5000rpm? The line showing your error below is indicating the spindle line is causing the issue
• Does the machine move in XY? IT should move in XY prior to trying to perform a Z move (after the spindle has turned on)
• Have you set the work offset correctly on your machine? Your code is G54, so ensure you have enough XY travel from the position you set this work offset to 

[eisenmanguitars]

Hi George, thanks for your time.  The machine moves as it typically does, prior to pressing play on the program.  I home the machine, then I bring it to zero, then I raise Z a few steps to give some clearance the way I always do.

The spindle is just a router with a manual wheel on it, so it is not programmable.  I turn it on manually.  I haven't run into this being an issue before, I've never adjusted spindle speeds for projects, only feed rate.

The machine jogs in XY and Z just fine prior to starting the program.  Once the program has started, it moves up in the Z axis as its very first move, then limits.

I believe I have enough XY travel.  The piece is well in from the X and Y limits of my machine.  It's the area of the bed I typically machine in.

Thank you!

[eisenmanguitars]

I have tried several things, but the same problem keeps occurring.  Here is the lates info from UGS:

>>> G0X1.095Y-0.1297
>>> Z0.6
>>> G1Z0.2F40
>>> Z0.0894F13.33
>>> Z-0.0375
>>> X1.0949Y-0.13Z-0.0403F40
>>> X1.0948Y-0.131Z-0.0429
[Error] An error was detected while sending 'G0X1.095Y-0.1297': (ALARM:1) Hard limit has been triggered. Machine position is likely lost due to sudden halt. Re-homing is highly recommended. Streaming has been paused.
>>> X1.0945Y-0.1324Z-0.0453
[MSG:Reset to continue]

[seth.madore]

Could you share your Fusion file here, and what post processor are you using? You mention UGS, but that's your g-code sender, right? What post are you using to create the g-code from Fusion?

Have you previously run Fusion toolpaths thru your machine?

[eisenmanguitars]

Hey Seth, thanks for your attention to this!  I've attached the file.  I right click on my toolpath, then select post process.  At that point I'm using GRBL, I hope I'm answering your question.  I have run many toolpaths on this machine through fusion, in this way (seemingly).

[seth.madore]

and could you share your latest g-code file here as well, that will help me to determine what's going on

[seth.madore · Accepted solution]

I suspect it's the G28 line at the beginning. If you change your "Safe Retracts" to "Retract Height", does it work then?
Note: you will have to manually insure that the tool is above the stock before hitting the start button

 

[eisenmanguitars]

Sure!  Here it is.

[eisenmanguitars]

That did in fact get it to start cutting.  What gives?  I've never had to change that before?  Also, I noticed on your screen shot that you are selecting output tool number, where I was not.  What is that?

[seth.madore · Accepted solution]

That (output tool number) was just a default setting in the post.

As to why you now have to select "Retract Heights", I suspect you were using a generic GRBL post and a recent update changed the behavior.

Do yourself a favor; safe a copy of the post to a local folder and use THAT post from now on.

[eisenmanguitars]

Thanks a lot for your help Seth! a little added bonus... After every toolpath operation (for a long time now) my router would always move up, limit out and throw a z alarm.  I always had to reset and home before making the next cut.  It doesn't do that anymore!

[seth.madore]

Awesome, good to hear!

[programming2C78B]

G28 is a common issue with the default GRBL post and the fact that A LOT of hobby cnc builders are not putting in a Z limit switch, so they turn the machine on then jog to find G54.

[simon.robinsonPUN8X]

Is this post still live as I would like to ask a similar question relating to Z height?

[eisenmanguitars]

Not active, closing now. Good luck with your issue!