arc output

[deckerc]

I'm posting code for my second time using X. I have a surfacing toolpath with the filter on. My code is coming out like so..

 

G2 Y-7.611 Z-14.165 R8.837

Y-6.117 Z-12.317 J0. K0.

Y-4.158 Z-10.917 J0. K0.

Y6.117 Z-12.317 R8.92

Y7.611 Z-14.165 J0. K0.

 

my machine alarms out at this point. the alarm has to do with I's, J's and K's. It is a fanuc control. How can I get the post to stop outputting I's J's and K's?? Tried looking in the post and in the control def. Think I looked too hard and confused myself.....

[Jimmy Wakeford from Barefoot CNC]

It is very strange to have j & k on one line and r on others. Look in the post for arcoutput and see if it is getting switched during posting and if so why.(ie. large or small radius, plane, over 180 deg sweep.)

[deckerc]

I agree, it is very strange.

this is the generic 3 axis post that came with X.

I can't seem to find any settings that would do that, but I suck at posts

[Jimmy Wakeford from Barefoot CNC]

put it up the the ftp and I'll take a look. You happen to be in luck, I am doing a post class right now and may use it as a project.

[Paul Decelles]

Looks to me like it is attempting to output arcs in the XZ plane without changing to a G18. Zip2Go the thing, send it to me and I'll take a look.

[deckerc]

I sent you an email, no access here. When I post the toolpath it doesn't start doing this untill approx line 161 or so.....

 

Thanks for taking a look

Corby

[deckerc]

Paul

I sent you an email too, it is putting a G19 (YZ plane). I only pasted the section of the program where the machine alarmed out, which is also where the first j's and k's came out.

 

thanks

corby

[Paul Decelles]

I haven't received the email yet, but while it is working it's way through the system, check the control definition settings for arc output. The new Generic posts allow for seperate arc control for each plane (ie. XY, XZ and YZ). Make sure you don't have one set to Radius, and the others set to Absolute (which the Fanuc will not read. You need to use "Delta start to center" for IJK output on a Fanuc). The post will force IJK output if a helix arc is detected (even if you have it set to output R's), which is exactly what happened in V9.

[deckerc]

they are all set to radius. I am playing with the arc error settings in the last box on that page now. If I check them all I don't get J' and K's. I'm trying to narrow it down now to which one is causing this

 

edit:

never mind, it was just putting them further down in the program

[deckerc]

I set all the arcs to "delta start to center" and the program ran. Hopefully someone figures out how to get all radii.

[Paul Decelles]

I still have not received the email. Can you send me the .mcx itself? ([email protected])

[deckerc]

Pual,

I sent the e-mail

 

I have since changed the control def to output only I's J's and K's and then switched to a parrellel tool path. thought everything was good until my tool and holder buried itself in the part. Thank god it was only aluminum.

 

time for a beer or 6....

 

 

Thanks for looking

Corby

[Storkman]

Actually, I ran into that same problem last week. Had all the arc planes set to radius and got 0's in the I's, J's, K's on a helix. I switched the arc planes for XZ and YZ to ST/CTR and it was fine. Funny part is I just went back to that file and switched them all back to radius and it posts out fine now.

[Jimmy Wakeford from Barefoot CNC]

no mail either

[deckerc]

Time to give up today.

 

I can't even get my e-mails to go thru today. I sent them again. If it doesn't work this time I'll back up ten yards and punt (tomorrow).

[heavychevy2155]

could the filter setting be doing some funny thing

[Jimmy Wakeford from Barefoot CNC]

if you look down in your postblock "parc" arcoutput$ is being changed according to what plane your in. You can take a look at mpfan's parc and fix your post, but someone went through quite a bit of trouble to set up the plane thing in post for some reason. make a copy of post before changing and let us know how its going.

[deckerc]

That is the generic post that came with X. I saw that section but got lost real quick trying to decipher it. I'll look at the mpfan...

[Paul Decelles]

Don't bother looking at the post, the issue is with the change in the way MP handles arc output based upon the control definition setting. If you have CD set to output radius values, the I,J and K values are not output. I'm working on a modification to the post to handle changing the arctype$, arctypxz$ and arctypeyz$ values when helix arcs are encountered (which is where the problem lies in your file - the filter is creating helix arc motion in the YZ plane). You will encounter the same issue in any MPFAN based post due to the logic that is forcing IJK output when a helix arc is encountered. I'll post again when we decide upon the best solution. For now, if you are running the new Generic post, set the XZ and YZ arc output to be Delta start to center so you get good output. If you are running an updated post based upon MPFAN, the linkplnvar$ variable is initialized so the XY plane control is the only one effecting output - I would suggest setting it to Delta start to center.

[mman10]

Paul,

I tried what you suggested. I also switched it to a parrellel toolpath. About 250 lines into the program it tried to wrap around the bottom of my part. I have break arcs on quadrants. The tool tried to go 37.5mm (1.5inch) thru my part. Like I said it looks like it's trying to wrap around the bottom side. I can't see this anywhere in backplot or verify. I'm guessing the simple solution for now is to not run the filter?

 

Corby (AKA Deckerc)

[deckerc]

For anyone interested in my solution to this.

I ended up modifying my post in parc section so there is no i, j , or k output only radii.

 

My control def is set to put out Radius only and now my post doesn't give it a choice either. I test ran my part using Flowline and Parrelel and all looks good.

 

thanks for the help guys!

 

Corby

 

Big Ben says What's a sophmore jinx????