surface finish parallel

[gary dunn]

for some reason, but only sometimes, when i do a surface finish parallel, mainly on very small groups of surfaces with a 1mm ball nose

end mill, the toolpath on the screen looks

okay but the output in the machine adds

a bunch of large loops and arcs. its really funny looking. this only happens when i

post at 0 or 90 degrees. when i change the

angle to anything but 0 or 90, it doesn't happen and the output matches the screen.

has anyone else ran into this ?

[Allan]

Sounds like you have arc issues in your post

turn off the filter, create arc function. Try it again. Are your arcs out put as R values or with IJK. I've seen this happen with small arc moves and R values. Try changing to posting with IJK values.

[lynnz]

The loops and very large arcs are a problem we have encountered. They are output as IJK in post. It has happened in more than just parallel toolpath. I just turn arc filtering off so we can run.

Out of curiousity, gary, are you running a Hurco? This is what we run and have noticed this problem from 7.2 on. We run 8.1 now.

Interesting that you can change angle to anything but 0 or 90 and its ok. I have seen it on projecting lettering onto a curved surface also.

lynnz

[This message has been edited by lynnz (edited 03-29-2001).]

[gary dunn]

actually, it's a Bostomatic.

i already have arc turned off and the post is set to not ever use canned cycles of anykind. strictly point to point.

that's what i am saying. it's real funny looking. occasionally i will get a machine error that says something like arc output error. i forget what it is.

 

[Ambassador]

lynnz;

The reason that it is only seen in 90 or 0 is because there are only 3 settings for arcs G17 G18 and G19. 1 degree to 89, there are no arcs. Make a small parallel file at 0 or 90 then copy it and change it to 1 or 89 then post them out with different file names. You will see the difference in the G-Code right away. The file at 0 or 90 will have a G18 or G19 and IJK's or R's while the one at 1 or 89 won't have either. Of course, the surfaces that you are cutting cannot be flat....

Ambassador

[This message has been edited by Ambassador (edited 03-29-2001).]

[Allan]

Gary, "strictly point to point", would give you no arc errors because it would be point to point. If you truly want point to point change linarc : 0 to linarc : 1, if linarc is not in your post then add it in the format linarc : 1.

[gary dunn]

linarc : 1 ... i'll try that.

[beav700]

Hi Lynnz.

Did 8.1 fixed the problem? We have 7.2 and eight Hurco machines. As you can imagine, we have the same problems with arcs that don't show up in Verify but do show on the control.

Turning of the filter works, but it creates very long programs that take all the memory and long time to laod.

[cadcam]

sounds like the post to me.

contact your MC dealer to have a look at it..

or send me the file so i can see if i can duplacate the problem.

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

jay/ aka cadcam

Precision Programming

cnc programming &

Predator reseller

email: [email protected]

web: www.ppcadcam.com

[Jim from Eastech]

If you are using the Mphur.pst, search for the note on 'swg18'. The hurco and boss controls reverse the G18 plane definition from what the rest of the industry uses. Set 'swg18' to 1 from 0.

[lynnz]

Finishline,

Switching swg18 to 1 did it. I had contacted my dealer a couple of years ago on this and was told it was a Hurco machine problem, so I had just switched arc filtering off ever since. Thanks a bunch.

This forum is great!!!

beav700- change your post and shorten them programs. Worked for me.

Lynnz