Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Tools are not coming down to the Z0 specified

17 REPLIES 17
SOLVED
Reply
Message 1 of 18
martinwiggall
526 Views, 17 Replies

Tools are not coming down to the Z0 specified

So, I'll include a few photos, videos, and my program code in this thread, but TLDR: I have a short simple program. I've quadruple checked that my (singular) tool is touched off, and that my heights are correct in the adaptive toolpath settings. Even though everything appears to be correct and the sim shows cutting the part, when I move to the Haas VF2 we use, it hovers about .3 ish above the part and cuts air. Even when going to the position screen, it shows the Z height as ~.3 as it cuts air, so the machine knows it isn't touching the part. I have no idea why. I'll include a text editor file of my G-code and a video of the machine shortly 

17 REPLIES 17
Message 2 of 18

I was going to attach a video but apparently I can't, so here's the .nc file 

Message 3 of 18
seth.madore
in reply to: martinwiggall

Would you be able to share your Fusion file here or privately?
File > Export > Save to local folder, return to thread and attach the .f3d file in your reply. To share the file privately, it's the same process, but email it to me: seth DOT madore AT autodesk DOT com


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 18
seth.madore
in reply to: martinwiggall

Looking at the backplot of your NC code, it appears that you may have your WCS origin set to the bottom of the part?

2023-08-07_10h03_33.png


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 18
CNC_Lee
in reply to: martinwiggall

@martinwiggall 

The movement you are seeing is correct per the g-code file you posted. Check that your Setup WCS Origin is set to "Model box point" and not "Stock box point" and also that the selected point is at the top of the part..

 

 

If my post answers your question, please use Accept as Solution.

CNC Lee
Fusion 360 CAM Post Processor Expert
https://linktr.ee/cnclee
Message 6 of 18
martinwiggall
in reply to: CNC_Lee

 It is set to model box point and is in the direct exact center of the part, which is where I always put my WCS...

Message 7 of 18
martinwiggall
in reply to: seth.madore

DAMNIT I didnt' mean to click "Accept Solution"

 

that WCS is from when I originally sketched the part, not my setup origin. my setup origin is in the center of the part

Message 8 of 18
seth.madore
in reply to: martinwiggall

I have the ability to Remove Solution 🙂

 

 

Can you share your Fusion file here? Instructions are above


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 18
martinwiggall
in reply to: seth.madore

Please do 😅 So, the WCS you are showing in the picture you attached is from when I sketched my part, that is not the WCS I specified in my Manufacture setup. 

Message 10 of 18
martinwiggall
in reply to: seth.madore

Okay, one moment 

Message 11 of 18
martinwiggall
in reply to: seth.madore

Here we go. I don't mind to share this publicly, it's a little homebrew project to make myself a versatile little hss toolholder. this file only represents operation one because I am on Fusion for Personal Use (used to have the Student edition when I was in trade school, and it lasted a little while after, but now it's expired 😞 haha) and therefore can only post process one tool at a time, no toolchanges allowed haha. Here it is! If I did somehow screw up the WCS simply by having it in a different place on the Design tab, please explain to me why that is, if possible, haha 

Message 12 of 18
seth.madore
in reply to: martinwiggall

Why would you set your WCS to a location that you can't access? Explain your method of defining your WCS at your machine.

 

Typically, folks will use either top of model or top of stock for 3axis purposes, or some folks prefer to use bottom of stock (top of fixture jaw for example).


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 13 of 18
martinwiggall
in reply to: seth.madore

It's never been a problem before. I have tons of other .f3d files that worked just fine with the WCS in the exact center of the part.. When I touch the tools off in the machine, the Z0 is set at the top of the part. If the machine thought the Z0 was deeper into the part, it would cut *deeper*, not cut less as far as I know..? I mentioned earlier, the tool is hovering almost half an inch above the part and "cutting air", and the toolpaths in Fusion do not reflect that. In the sim in Fusion, it appears to cut correctly, no?

 

TLDR: does it matter? 

Message 14 of 18
seth.madore
in reply to: martinwiggall

The distance from the center of the part (WCS location) to the top is .375. You then (at the machine) set your WCS Z0 to the top of the part. This effectively raises all your tool Z depths .375". It will always cut less, not more.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 15 of 18
martinwiggall
in reply to: seth.madore

also if you literally mean setting up WCS at the machine, it's probably what you think it is. 

 

edge find the part, find center of X and Y, offset, part zero set. no Z offset. 

touch off tool with piece of paper. offset, tool offset measure. 

Message 16 of 18
martinwiggall
in reply to: seth.madore

I'm going to tentatively accept the solution, you probably know what you're talking about. I'll give it a try and be back in a bit, my laptop is slow

Message 17 of 18
seth.madore
in reply to: martinwiggall

You can continue setting your WCS to the center of the part (it just makes more work for you and can be error prone), you'll just need to manually subtract the distance from top of part to center (where you set the WCS in Fusion). Again, error prone and just generally should be avoided.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 18 of 18
martinwiggall
in reply to: seth.madore

I just now got everything posted and I'm about to try it, but I think I realized what was going on in my head. I haven't been doing this for a long time, been out of trade school for a year-ish? and I haven't written a program in a hot minute. I think I was confusing the way WCS is set up on a cnc lathe versus how it is set up on a mill. Be right back 

 

Edit: All appears to be well! The program still hasn't finished, because with Fusion for Personal use, you don't get any rapid movements between cuts, so it takes significantly longer than what the Machining Time would suggest. But I believe we're good! Thank you!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums