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: 

Fusion posts code that throws a 3.316 alarm on Haas VF3

9 REPLIES 9
SOLVED
Reply
Message 1 of 10
ernieR8HAW
361 Views, 9 Replies

Fusion posts code that throws a 3.316 alarm on Haas VF3

I have set up a job on one of the Haas VF3 machines this morning. I set the tools, ran the work offset templates, put a plate on the table and did the work offset cycles for X, Y and Z. All looks well there.

 

The control is throwing a 3.316 Z overtravel alarm on this code and I do not understand why.

 

I must not be seeing a problem with the code that Fusion has posted. I have the snipet copied below. I looked for a modal G52/92 and there is none. I have the G19 for the lead-in move and the J and K look good to me.

 

 

(First Operation: Face Bottom Side.)

 

(T13: 3.0" Face Mill, D=3.000".)

 

(Safety Start)

 

N09 G00 G40 G49 G80

N10 G90 G94 G17

N15 G20

N20 G53 G0 Z0.

 

(Face Bottom Side.)

N21 M1

N25 T13 M6

N30 S7000 M3

N35 G17 G90 G94

N40 G54

N45 M8

N50 G0 X14.6935 Y8.2

N55 G43 Z0.6 H13

N60 T3

N65 G0 Z0.3

N70 G19 G2 Y7.9 Z0. J-0.3 K0. F25.

N75 G1 Y6.5

 

I was wondering if you could see some problem that I am missing in the code. The line throwing the alarm is block N70. Am I wrong having the incremental Z coordinate of the circle center for the lead-in interpolation at K 0.0? This line brings a shell mill down to Z 0.0 to face the plate, so I should be correct landing it there.

 

Either there is something I am not seeing or there is an issue with the machine.

 

 

 

9 REPLIES 9
Message 2 of 10
seth.madore
in reply to: ernieR8HAW

Couple of questions:

1) What's going on after that snippet that you've shared?

2) Does the code run if you (in Fusion) set your Vertical Lead In/Out to zero?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 10
ernieR8HAW
in reply to: seth.madore

Seth,
In Fusion the simulation looks good. It runs without a hitch. But the machine does not like this code for some reason. It acts as if there were a G52 still operable somewhere and the offset were putting the tool outside the envelope. But this is certainly not the case. Also, I have run my tool and work offsets multiple times and they always come out nearly spot on.
This is a program I use to cut the basic version of my 1.0" X 12.0" X 30.0" fixture plates. I qualify the back face, turn the plate and qualify the front face and then do a series of drilling and boring ops.
I will set the vertical lead in/out to zero as you suggest and see if the simulation also runs in Fusion. I will report back soon.
Thank you for getting back with me. I was not expecting much from a forum as my past experience with them has been less than stellar.
Regards,
Ernie
Message 4 of 10
seth.madore
in reply to: ernieR8HAW

Oh, I expect everything to run quite well in Fusion, it's at the machine that I'm asking about (in regards to removing the vertical arc moves)

 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 10
ernieR8HAW
in reply to: seth.madore

Seth,
Just got back from the machine.
In the below snippet the machine now throws the same 3.316 code at block N60.

(First Operation: Face Bottom Side.)

(T13: 3.0" Face Mill, D=3.000".)

(Safety Start)

N09 G00 G40 G49 G80
N10 G90 G94 G17
N15 G20
N20 G53 G0 Z0.

(Face Bottom Side.)
N21 M1
(Face Bottom)
N25 T13 M6
N30 S7000 M3
N35 G17 G90 G94
N40 G54
N45 M8
N50 G0 X14.6935 Y7.9
N55 G43 Z0.6 H13
N60 G0 Z0.2
N65 G1 Z0. F8.
N70 Y6.5 F25.
N75 Y-6.5

I was half expecting it to run with no problems.
Alas ....
Any further insight at this point?
Ernie

Message 6 of 10
seth.madore
in reply to: ernieR8HAW

That makes no sense. You do have a value in H13, right? And your have properly set your G54 Z shift (if needed, unsure how you touch off tools).

Looking at your active G codes, is there anything that's jumping out at you? It almost feels like it's gotten into a state it doesn't like. This is cliché, but could you try turning it off and back on again? (this will set all g codes at default values)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 10
ernieR8HAW
in reply to: seth.madore

Seth,
It does not make a great deal of sense to me either. But then I have only been doing this job for a bit over a year. About two years ago I left a long career at sea and was looking for something else to do as I enter my "golden years". So, a programmer or a machinist ... I am not. But I am learning as much as I can about both.
So, I can not see anything in the code that is amiss.
We run 27 Haas machines at the shop. They are all equipped with the WIPS system and so I use the probe to set my tool and work offsets. It has always worked fine for me. This particular VF3 had been serviced last week and this is the first project that I have put on the machine since then. The system was recalibrated by the factory technician. Of course, I also ran the recalibration yesterday in preparation for today. He had the system spot on.
I set the machine up and ran the tool and work probing macros and they wrote to the registries with reasonable values. So, I believe the tool length offset number H is accurate.
I will go out and shut the machine off and then restart and try to run the last version of the program without the vertical lead-ins and report back to you.
Best,
Ernie

Message 8 of 10

Hello ernieR8HAW

 

Not being able to see your set up but I might imagine it's a plate on the table. I would venture to guess the overtravel might be real. You might have to set the tool farther out in the holder or use a longer holder. You can just move your Z offset up about .2 and run it above the part to find out.



Bill Cain
Sr. Technical Consultant
Message 9 of 10

That's a good point, I didn't consider running out of travel in that direction


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 10 of 10

Bill,

 

You are absolutely correct. This problem was simply a matter of the tool/tool holder not being long enough. It is nothing to do with the post.

 

I am coming to this job in my "golden years" as a third career and it is always a bit discouraging to see with what complete composure and self-assurance I continue to step into all the rookie mistakes.

 

Thanks also to Seth for his extended assistance. You guys have been great. This answers my question.

 

Best,

 

Ernie

CMI

 

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

Post to forums  

Autodesk Design & Make Report