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: 

Machine Stops on Z Axes Soft Limit

17 REPLIES 17
Reply
Message 1 of 18
Latheboy
434 Views, 17 Replies

Machine Stops on Z Axes Soft Limit

Hi all,

 

Odd situation during a program cycle. I am making a rectangular part with full plunge depth of cut of .300. The first tool does a radius of the 4 corners at full depth around the material in .030 step overs in a total of 10 clips of each of the 4 corners lifting Z to 0.00 and then back to -.300 for each pass. 

During the 4th or 5th pass, when the Z axis is dropping towards -.300, I get a Z axis soft limit overrun at -.260  this makes no sense to me. 

I looked at the code and don’t see anything odd and even tried to re post process which made no difference. Any suggestions?

Thanks

 

17 REPLIES 17
Message 2 of 18
a.laasW8M6T
in reply to: Latheboy

Most machines will look ahead in the code and give a soft limit error before the line that actually will hit the limit.

 

my machine will say "-x limit 553" saying that line 553 would cause the overtravel but will do this several lines before that one.

 

without seeing the fusion file/NC code/knowing where your WCS is set, what type of machine/controller you have, post processor?

its just guess work to diagnose.

Message 3 of 18
Latheboy
in reply to: a.laasW8M6T

I have attached two scree photos.  One extracted from a video.  Is there a way to attach the .pim here?

 

Thanks

Message 4 of 18
Latheboy
in reply to: Latheboy

Here is a snippet of the code.  The referenced block is N5955.

Message 5 of 18
Latheboy
in reply to: a.laasW8M6T

Sorry for the multiple posts.  I realized that I could pdf the entire code.  Many pages, but all there.

 

Thanks for your help.

Message 6 of 18
a.laasW8M6T
in reply to: Latheboy

To attach the .pim files here you just need to change the file extension to .nc as the forum only allows certain file types.

I extracted the text from the pdf and ran it through NC Viewer and the line that seems to be causing the problem has an erroneous arc that i don't think should be there

alaasW8M6T_0-1705896087458.png

 

I assume you are just using the standard Fagor 8055 post?

 

If you could share the Fusion file here that would help.

goto File>Export>Save as .f3d/.f3z

Message 7 of 18
Latheboy
in reply to: a.laasW8M6T

I am not using the "standard' Fagor PP.  I have attached what I am using which was modified for manual tool changes (since I don't have an ATC) by another extremely helpful Autodesk person some weeks back.

 

I have also attached the part file as requested.  What I neglected to mention previously is the line where the code stopped running and stopped the machine seems to be at the very end of the cycle where Z would lift .400 above the parts surface. 

 

The other issue is that not all of the material was removed per the design/programming, meaning that I believe that it had further to go to complete the first operation.  I understand that the CNC reads a number of lines ahead and maybe this is it, but I believe that it had two or more passes around the entire part to finish which seems like a lot of code.

 

Thank you,

 

Steve

Message 8 of 18
a.laasW8M6T
in reply to: Latheboy

I've had a look at the setup and the posted code you have attached here and I posted again from fusion and I cannot find any issues with the program at all, everything seems fine in terms of Z heights.

 

I see you have a large number of NC programs in the browser, I suspect you are creating a new one every time you click post process. the Idea with NC programs is you only create one then you can select the NC program and click post from there.

 

Alternatively you can uncheck create in browser

alaasW8M6T_0-1706037911883.png

 

Might be worth watching the videos on NC programs

https://help.autodesk.com/view/fusion360/ENU/courses/AP-NC-PROGRAM 

 

 

Message 9 of 18
Latheboy
in reply to: a.laasW8M6T

Thanks for reviewing everything. Did the “arc” concern go away?  I will eliminate all of the NC programs and watch the video as well. When I ran the part A (front of part) it ran perfectly and I still had all of those NC programs. 

I will try it again and hope it runs the entire part. 

thanks

Message 10 of 18
a.laasW8M6T
in reply to: Latheboy

yes the weird arc was gone.

 

The multiple NC programs aren't really a problem as such, its just not the right workflow and messy seeing lots in the browser.

 

I don't use NC programs at all as that's my personal preference, but they do have their place.

Message 11 of 18
Latheboy
in reply to: a.laasW8M6T

I havent been able to try to run the program again, but I do wonder what is causing the Z soft limit and machine stop?

Message 12 of 18
Latheboy
in reply to: a.laasW8M6T

I cleaned up the NC programs as suggested.  I re-posted the file and ran the part with the same results.  I Have triple checked everything and don't see a reason that the machine is stopping in the same place and shutting down.  Not sure if anyone sees anything here, but I am posting some photos at the machine in hopes that you see an issue in the setup.  I have run the same part on side A numerous times without an issue, so I am baffled here.

 

Thanks,

 

Steve

Message 13 of 18
a.laasW8M6T
in reply to: Latheboy

Hi

 

you say this is a knee mill?

How is the Z axis controlled? is it raising the knee or does it drive the Quill up and down?

 

Maybe you are just actually running out of Z travel in the OP 2 setup.

Does it sit lower in the vice than OP 1?

Maybe manually run the z axis down off to the side of the part with that tool to see whether that is indeed the problem

Message 14 of 18
Latheboy
in reply to: a.laasW8M6T

It is a knee mill.  The position of the quill is at Z 1.75245 at machine home, and home is 0. 

 

At Z 0.00, the quill reads -1.75245 and the tool tip is touching the material/part.  The programmed depth of the cut is

-.300, so the total depth is -2.05245.  The Z axis can still move down an additional 2" before hitting the end of travel.  This is what is so confusing.  I have the same exact setup for the 2 op and the knee remains in the same locked location.  The second op is simply cleaning up the perimeter previously held by the vise, then a chamfer of the perimeter and holes drilled and tapped during the first op. 

 

From the top of the part "0" (-1.75245 from home) , I went to MDI and entered  Z-1.6 and the quill moved down an additional 1.6"  If I tried with Z-2.5, I get the axis limit error which prevents the move.

Message 15 of 18
fredsi
in reply to: Latheboy

Steve,

 

Set the VERTICAL leading(s) to 0in. and see if the code then runs without stopping.

 

Fred

Message 16 of 18
Latheboy
in reply to: fredsi

HI Fred,

 

I wish I could say that I understood the reasoning behind the solution, but that resolved the issue with no other changes.  Can you explain how this changed the result?  I went back to OP 1 and the same vertical lead of .05 is there and that side ran just fine.  Very confusing Thanks so much.. 

Message 17 of 18
fredsi
in reply to: Latheboy

Steve,

 

Reason the 0.05 entry on first tool path didn't cause a problem is - it was ignored. Since a ramp into the part (helix) was specified, there was no need to honor the vertical lead-in. Thus, no G19 was output in the code; it was only when it came time for the finish pass that the vertical lead-in was honored and resulted in a G19, which ended up confusing the controller. 

 

As I mentioned in another post, since you can always helix in, ramp in, zig-zag in, or whatever, I don't think the vertical lead-ins are that useful and can be defaulted to 0in. to avoid all the plane switching codes (G17, etc.).

 

Fred

Message 18 of 18
Latheboy
in reply to: fredsi

Fred,

 

That makes great sense. Thanks again. 

Steve

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

Post to forums  

Autodesk Design & Make Report