I use a 2" diameter surfacing bit for most of my facing operations, it would be super helpful to add a fourth option here that would allow me to measure its height using the corner finder on the spoilboard. It won’t fit over the corner touch plate without colliding with my spoilboard’s corner, and jogging it down to the spoilboard has to be less accurate than using the corner finder as I did before.
Image of current options when a large tool size is mtc’d:
I also notice that this dialog pops up for .5" diameter tools, seems unnecessary.
Found an issue with the post processor: The machine moves to home when using g53 safe retracts regardless of whether the move to home at end is selected.
Resulting output at end of the toolpath, I don’t think G53 G0 X0 Y0 should be included, just g53 G0 Z0
Also noticed something odd with the second tool change in this toolpath, it seemed to disregard that it needed to change tools and gave me a spindle about to start warning instead of going through the tool change process similar to the last tool change. I will be posting my files individually tool by tool for now until I can be sure its not going to start cutting with the wrong tool.
The previous tool change called T42 as it should have:
Not sure why it would post correctly on one part of the toolpath and incorrectly on another.
Ok, looks like we have a couple of issues here, starting with the big slabbing bits:
The reason you’re seeing that pop up is because you’re trying to measure a large slabbing bit… but you knew that… theres some additional logic to it:
If your tool height offsetter is ABOVE the work surface you won’t see this warning if you have a tool that is .75" or less in diameter. If it’s BELOW the work surface you’ll get this warning if you have a .4" or larger tool. This is because in some setups the tool height offsetter can not only be below the worksurface, but VERY close to it. We wanted to make sure users bits were’t smacking into their work surface before hitting the touch plate.
If you’d prefer to not get this pop up everytime you try and measure a large tool you can do an MTC and just “touch off” the tool right to your work surface anywhere you want.
Tell me more about this corner finder? That would seem to only do XY, is this some kind of a Z touch off device you’re talking about?
Post processor:
Are you using our EX post or another Centroid/Mach post?
You shouldn’t get a G53 move at the end of a job if you have your post options set like this:
(we do however have a “move to home” command in our M30 that you can toggle on/off in the wizard)
That incomplete tool change can be solved by making sure that “USE M6” is on (should be by default)
Yep, my THS is set below the work surface, mounting it above seems like it could cause collisions working near that corner. My spoilboard is 1.25" tall so mounting it above doesnt appear to be an option without a custom mounting solution.
I would like this dialog to pop up for only my 1.5" or higher tools, can this value be made to be adjustable?
Yep, I just think using the auto z-corner finding touch plate would be easier and more accurate than manually jogging down.
I am referring to the auto z-corner finding touch plate sold by you all.
I am using the standard EX post with rotary mounted in X
Here are my post settings, I had m6 checked. Tried re-posting, same result below:
There’s no exposed setting in the wizard that can be edited. In theory you could it by editing the tool change script, but that’s getting into the danger zone.
The plate could be used for manual measurement, but we decided to not offer this option because most people in this situation (folks with tools that are truly too big for the tool height offsetter) couldn’t fit them in the touch plate anyway. Then they would be in a situation where they would need to bail out of a job…
Here’s my recommendation:
The tool height offsetter is very accurate. I’d use that if you can. if you can get your slab bits to fit on it by jogging around in XY that would be the best way. If you don’t want to do this during a job just use the MTC button ahead of the job, and run the job with no tool changes…
I’ll take a look at making that value adjustable.
For Fusion, are you using our machine profile and our post that you downloaded from our site?
Yep - using your post processor from the website. I sent the file over to Leire, I assume you can see all the open support tickets? If not please send me your email and I will forward it to you.
Yeah I may be able to get the touch plate to work, just have to move my default touch off location further into the corner or just get a smaller surfacing bit for ease of use.
Thanks, having that setting as adjustable would save me some keyboard input time.
Are you also using the machine profile? You need to use both. It’s in the video here:
https://www.avidcnc.com/support/instructions/software/downloads/fusion/
If you still see this issue please post your file here (or email it to me) as I don’t have direct access to support tickets.
Yep, using both.
What is your email?
Are you actually doing a rotary job? If you aren’t you need to use the 3 axis machine profile
I figured it would be able to handle both - I switched the machine definition and still getting this:
Can you send me a download link for your file? Or post it here?
You can DM me directly if you’d prefer not to post it publicly
Sent it to your dms, have to be very protective about my files these days.
Totally understand. I’ll keep it private
Hey Greg, this one was a bit of a needle in a haystack, but I think I solved it. It will require a new post (which I will attach below)
This issue was isolated to only files with 4th axis work in it.
Make sure you have your post set like this:
It should be noted that you CANNOT use rotary with anything other than G53 safe retracts, but you CAN use it with a “no move” at the end.
And for some additional clarity:
The “no move” at end means that FUSION will not issue a move command at the end. Our M30 script WILL do a move command at the end of a job. No matter what it will always to a G53 Z0 home.
It will move to XY home if you have that set in the wizard.
Avid CNC EX Router V2.cps (77.2 KB)
Try this post to see how it works
Thanks Eric! Appears to have fixed the issue with moving to xy home! The issue with missing tool change #2 persists, still does the first and third tool changes correctly.
Yes- good catch. Should that be disabled on all tools for the post to work properly?
Appears to work!
Yup! Even though you might be “manually” changing the tools it’s really an ATC without a tool rack. So set all of your tools to NOT be manual tool changes and you should be good to go.
