Help !!

[kathy]

Another Crisis!!

I am machining a part where the (2D) profile is mostly arcs, on our Fadal (using Fadal format code). Mastercam output the code as a series of arcs. The machined part is noticeably ‘jagged’ – out by at least a quarter of an inch.

I’m climb cutting the pre-dominantly CW profile, and the code has short G2 moves (with very large J values) with G3 arcs and negative J values. I would include a sample here but I want to save space. I have a packet of file ready for e-mail if someone wants to take a look. I have tried different filter settings without getting the code to change.

The code looks fine when viewed by Metacut – the profile is smooth. I’m trying to get the profile machined on our Fanuc controlled machine, to see if it is a controller issue.

Our Shop Supervisor had me re-program the profile in SmartCam – that’s his solution – to go back to using SmartCam! No wonder us programmers are grumpy!

Thanks for help in advance!

- Kathy

------------------

Kathy Richardson

Applied Aerospace Structures Corp. (AASC), Stockton, CA

phone: 209-983-3203

fax: 209-983-3375

website: www.aascworld.com

[gmenzies]

we use metacut and meta view and a fadal. if you are using metacut. then most of your code should be liner moves and then filtered through metacut for arcfiltering. if you are using metaview. i would assume you are doing 3d machining.

if you are machining a surface , then it could be a cut tolerance issue. try increasing the default tolerance from .001" to .0001" also the fadal we use , on a yz or xz arc the g18 or g19 must be in place . this tells the control what plane to cut the arc.

 

[gcode]

kathy,

on the contour page there is a drop down

labeled "Roll cutter around sharp corners"

The choices are "none", "sharp", and "all"

Experimenting with those settings has solved similar problems for me in the past.

 

[kathy]

Thank You,

gcode - I tried changing my settings for 'roll cutter...' and the code didn't change. I tried different setting on my filter - nothing.

This is a simple 2D contour around a part. I have a trial version on Metacut view to see if it would help up in other ways. I can't find the 'arcfilter' function.

I wold be glad to send an e-mail package to anyone willing to take a look

Thanks, Kathy

[Toby]

Kathy,

Are you running real close to your machine travel limits?

------------------

Toby Baughman

Magic Mfg

[Carl Vallance]

Kathy, I've had similar problems with our Fadal when using cutter comp in the control. It seems to be a bug in the Fadal. My work around is to turn cutter comp off in the control and on in the computer. I'm not sure you are having the same problem but it sounds like it. E-mail me your files and I'll see if its the same on my mill. [email protected].

[gmenzies]

metacut and metaview are two differant programs.

view is about $350.

cut is about $2000. its a optimization program

we do our cutter comp in computer. when we need cutter comp for fitting we set to both and adjust diameter offset in incremental :ie

-.002 will cut .001 per side

[shipster]

Had this similar problem before and we would convert to spline data and change the number of control points to get the best result.

[Kenneth Potter]

 

Go into setp & check your tool table setting Dia or rad ?. & your CRC mode,normaly "M96" intersectional CRC roll off(default)

hope this helps

Kenny

[camguy]

Kathy, send me your files, i would be interested in looking at your problem

send to [email protected]

Steve

------------------

 

[kathy]

Shipster,

How do I convert my chain (of arcs) to a single spline? I tried to convert the chain, and all I got was a series of splines instead of arcs.

This is an approach that sounds logical.

Thanks to everyone for the cutter comp suggestions, however, we don't use cutter comp at the machine control.

Thanks, Kathy

[Ambassador]

Kathy/Carl are you using cutter compensation? I have seen a problem with Fadal's where if you Modify, Fillet the machine heads off in the wrong direction or cut's the arcs backwards. If you "refillet" between 2 arcs using Create, Arc, Tangent this should fix this problem. Although the same "nci" file posted would run no problem on a Mits control.

Regards,

[camguy]

Kathy, I took a quick look at your files, and i notice that some of the arcs are very large, like close to 500. inch rads. some machines may not be able to resolve the math, causing it to lose position. I reposted the program with a selca post and it converted arcs grater than 100 in. to lines. you should talk to your dealer and see if you can get your post modified to do the same. its under program switches: maxrad :100. Converting your geometry to splines should work, in the case of this part you should create three separate splines, one for the bottom profile, left, and top. this will increase the file size considerably. We are shutting down for Christmas today, so i won't be able to look at your files again until the new year. Hope this helps out for now.

Steve

[camguy]

Kathy, to create splies: create/spline/curves/chain/partial

select first and last entity on lower profile, make sure switch is set to delete to get rid of the arcs and lines. i just did it and ran a toolpath, and the file size was very reasonable in size as it was all lines, no arcs. be carefull when creating splines for machining, if you have too many control points, it can sometimes give you a bad toolpath. if the splines have a lot of shape to them, run the "remnodes" chook with the tolerance set to .005. this will smooth out the spline and reduce the toolpath size.

Steve

[kathy]

All of you guys, and this Forum, are just awesome!

camguy, thank you for explaining how to convert my chain to a spline - what ever I was doing before wasn't working.

Scott, thanks for the modified post - the code looks great, and we will be running it on the Fadal in about an hour. I'll let you know.

Happy Holidays to all. My vacation starts at 2:00 PM California time, and I will see everyone next year! Everyone stay safe!

- Kathy

[Allan Brown]

Allan informs me that this is a known issue.

Add this line to like this one to the post where arctype is initialized:

maxrad : 999.999 #Maximum arc radius

[kathy]

Hello All!

Tried the profile with arcmax limited to 999.99 and still had a problem. Talked to Fadal - found out that without cuttercomp, the arc limitation is 399.999! So I modified the post, and cut some more code - Mike will run it next week.

I'm almost an hour into my own time - so I'm outta here

Thanks, Kathy

[jeepman]

The 399.999 sounds similar to the xxxxor control we use, which is a Spanish control that aparently uses the metric system for its calculations. The manual said that max arc radius was 99.999. I found out that this was mm not inches. When I changed the max arc radius to about 39 inches my problems were solved.

[George Bailey from Warvel Products]

Kathy,

Another method for creating a spline out of arcs, is to create point along an entity, delete duplicate points, then create spline, automatic.

George

[Dino]

Kathy I ran into the same problem today. It turns out in the Fadal Operators book it says there is a maximum programmable arc radius of 399.9999! The I value for the g3 code was 544. something. way over the limit. The Fadal control compensates by feeding at a 45deg angle and then straight line. As it does in rapid moves. This causes the jagged moves. I'm looking for a solve either in MasterCam or my post.

[CycleTimeCharles]

There is a variable in the post called "maxrad" Set it to 390

[kathy]

Hey Guys!

I apologize profusely for not replying that my problem was fixed. In December! (it was the day before Christmas vacation….).

Yes, the solution is to set in the Fadal post:

maxrad : 390.999

Kathy