SP1 and post issue ?

[?Mark]

Still have the same problem as in original release, but not sure if it's post or MC issue.

Do we need to update posts again?

 

EX:

Draw a rectangle, fillet all corners, toolpath contour clockwise starting with a straight line, in toolpath parameters chose multipasses, finish passes 2, spacing 0, lead in/out with a line and tangent arc, enter on first cut, exit on last cut, post

 

I still get missing G1 code after arc move:

 

G2X-2.8637Y2.8536R.5

X.3557

 

Another thing.

Picking arc centers for helical toolpath won't let me specify dia I want to cut (blanked), it defaults to 1.0" arc dia. Is it supposed to be this way?

 

Kind regards, Mark

[SLJ]

Mark, I just tried it on one of my posts and can't find any instance where it fails to follow a G2 with out a G1. May be a post issue as you suspected

[?Mark]

I also happens when using generic fanuc 3x mill post that came with MCX

WTH???

 

 

Mark

[Jimmy Wakeford from Barefoot CNC]

Mark, I have been able to duplicate it by setting plunge feed same as cut feed. This is what's happening.

In plinout there the "`" if front of sgcode (`sgcode) tells the post to only output the gcode if something else is also coming out, otherwise hold on to it.

It does keep from outputting, but updates the pprv_gcode$ var which is wrong. I tested by doing:

code:

---

plinout #Output to NC of linear movement - feed

"JIM-test1",prv_gcode$,e$

pcan1, pbld, n$, sgplane, `sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, feed, strcantext, scoolant, e$

"JIM-test2",prv_gcode$,e$

---

For now you can take the "`" from in front of the sgcode or set plunge feed dif from cut feed.

[?Mark]

You're right Jimmy, setting a diffrent plunge feedrate fixes it, but you get an "ugly" line "G1F__;" between G2 and a next linear move.

 

quote:

---

For now you can take the "`" from in front of the sgcode

---

Isn't it going to give me a bunch of unnecesary repeats of G1's and G2/3's

 

Thanks very much for looking into it.

Kind regards, Mark

[Jimmy Wakeford from Barefoot CNC]

Yes it can I sent this topic to the post dept so they can get it worked out. This is also affecting prapidout.

 

Lemme think about it and I'll puty up some code to keep the g1 lines clean

[?Mark]

quote:

---

I sent this topic to the post dept

---

They might be already working on it

thread

 

Mark

[Paul Decelles]

It's a bug in MP that has already been logged. Wish I could give an estimate on when it will be fixed but it's virtually impossible to do so.

[?Mark]

Appreciate it Paul, at least now I know to change plunge rate to be different from feedrate and all should be good.

Are you also working on fixing the XY shift while rapid Z retracting?

 

Regards, Mark

[Paul Decelles]

Mark,

The .0001 XY shift on the Z retract has been logged and the developer is aware of it. Can't guarantee anything there either but I don't consider that to be a major issue.

[Hymen]

Thanks Mark for pointing me here!

In this post:

http://www.emastercam.com/ubb/ultimatebb.p...ic;f=1;t=017085

 

I brought up this same subject, with one addition.

The change in feed rate fixed my situation with alarming out. But, didn't fix the loops in engraving. I get loops on top and bottom of R's (one or the other) and so far on top of P's. Anyone else come across this? Got a fix?

Don't have permission for FTP or I'd put up screenies, code and the MCX file!

[Hymen]

update:

Change direction of chain, and loop goes away!