Printable View
i have a tormach 770 i just bought it has the path pilot . whenever i post with fusion 360 it spits out a M998 .This M998 seems to want to crash the spindle into the work piece . When i manually delete it the post is good . Is there a way for it to not spit this line of code out ?
I have no tool changer on the machine. They all need to be changed by hand.
You want it to move in Z axis only. There's no way to crash into the part if it only moves UP. Check a current manual Page 61 and 68. Here's the relevant bit from page 68:
G30/M998 Move in Z Only – The G30 or M998 G-code commands can be used to move the mill to a pre-set position. The position is settable using the Set G30 button on the Offsets screen. A G30 or M998 command is typically programmed right before a tool change line in G-code programs so that the spindle head clears the workpiece with sufficient distance to be able to change tools. When selected, this option moves to the tool change position in Z only, otherwise a coordinated XYZ move occurs on G30 or M998.
According to the manual, M998 and G30 behave identically on the Tormach.
The 3 vids here show everything you need to know
https://www.youtube.com/watch?v=a2iJ...EFpw-Px8dAxnEL
and if you do a search here there are a few tormach posts Inventor HSM & HSMWorks CAM - Autodesk Community
Looking at the tormach.cps, there is only one place where the M998 is added.
Do a search for "writeBlock(mFormat.format(998));" and either delete it or put "//" in front of it to comment it out.
I haven't watched the attached videos, but I'm sure they mention that after editing you should move the post file out of the webdeploy/production/xxxx/Applications/CAM360/Data/Posts directory or you can lose your edits with the next update.
Dave
Modified posts should be placed in: C:\Users\YourUserName\AppData\Roaming\Autodesk\Fus ion 360 CAM\Posts
Regards,
Ray L.
Quote:
Originally Posted by SCzEngrgGroup
Yeah, guess I should have mentioned that. And the caveat - Unless you're one of those MAC people...