Cutter comp control

[DavidB]

I saved the MCX file as a V9 file.

Opened the V9 file in Mastercam V9 created identical toolpaths using the same geom I did in MCX and V9 gives good toolpaths and backplot looks good.

I open this V9 file in MCX and backplot the V9 toolpaths and MCX's backplot gouges.

The posted code from V9 and MCX are the same. So I think it's just a MCX MR2 backplot and verify issue.

 

Below V9 toolpath

 

Below V9 file opened and backplotted in MCX MR2

Note the gouges!

 

[bhayden10]

I have a couple of Mazaks that have to use control comp. I have always had these same issues with it backplotting right. My reseller says it is a known bug but nothing can be done to fix it. It almost always puts out the right code though. I was dissapointed that it wasn't fixed in X. It sure makes it hard to program a part and feel good about it.

[Roger Martin from CNC Software]

quote:

---

So I think it's just a MCX MR2 backplot and verify issue.

---

David,

If so, please submit your MC9 file to [email protected].

 

Thanks for your input!

[Matt Berube at Ferron Mold]

quote:

---

My reseller says it is a known bug but nothing can be done to fix it.

---

Wow, that really underscores the importance of submitting the problems to [email protected] if your reseller isn't giving you the right answers.

[Fig sign]

I said it before and I say it now :

just do not consider me the Dumbass - compare your settings for toolpath accurasy and chaining tolerance .

I do not say it `s not a bug .

Simply I got bad results with ver9 too -just loose chaining tolerance a bit and you`ll see

[DavidB]

Its more than just a Backplot issue as I first thought the posted code witgh multi passes is screwed too.

The same toolpath posted with wear,computer oroff posts fine but the gouge you see in the X pic above is in the posted code when using comp in CONTROL only.

 

quote:

---

just do not consider me the Dumbass

---

Iskander,

I dont know why you feel like this?

I tryed your suggestions thank you.

In X all toolpaths other than CONTROL comp backplot and post correct, but simply changing the comp to CONTROL in the toolpaths screws backplot and the posted code. From what I tried in V9 with the excact same file and excact same geom gave good backplotting and good code.

I respect your comments and help greatly.

[ToolMan184]

Try and keep it from starting the contour in the middle of the start geom on the lead in lead out page. I have used comp in control on a fanuc control for years with no problems.

[DavidB]

 

I draw a 50mm square put 1mm corner fillets on all corners.

Toolpath contour outside and inside of contour with comp in Control.

The lead Outs give Inverse radius?

The lead In moves are not tangent to a 90 degree arc?

If I change the cutter comp to anything other than CONTROL toolpaths are fine!

[DavidB]

Question,

Why is my Backplot of a Toolpath programed with Comp in Control not backplotting on line but offset by cutter rad????

 

 

[DavidB]

I think I found the my problem in Backplot.

Config,Backplot,"Simulate Cutter Compensation" was ticked.

 

Unticking this gives a completly different toolpath.

[MMT-USA]

Can you post the NCI file for that one path giving you trouble?

[DavidB]

I have a toolpath with comp in control with multi passes which gouges on the second pass only because mastercam is out putting an inverse arc.

I run this toolpath in vericut and get this.

 

 

I've worked out my backplot problem in MCX it was "Show cutter comp" in my config

[gcode]

David,

 

at this point, I'd just post it with comp off and add the D offsets, G41's and G40's by hand.

Looks like Vericut saved the day.

[DavidB]

gcode,

Thank you very much for all your help on this file.

I sure owe you a few beers

 

What about the multi pass toolpath that gouges?

Will the responce from QC fix this? I will check also.

Or is there a bug?

[Fig sign]

In your part in ver 9

Change chaining tolerance to less accurate and you`ll get loops and googes too

[DavidB]

Iskander,

Everything in V9 was Identical to X.

Geom,Toolpath chaining Tol ect.

 

 

My backplot in X was screwed because I had "Show cutter comp" ticked in my config file. Backplot in X is OK now.

 

I sent the X file to QC Regarding multi passes with comp in control.

They replied with..

The linearization looks to be a control definition setting.

In the control def. look in the ARC section and make sure that “ENDPOINT CHECKS” is not active.

 

See the attached screen shot.

 

 

I will check my control def tonight and see if this is my problem and let you know.

 

Thanks

[DavidB]

My control file....

 

So the gouge in my toolpath is not because of my control config.

[Fig sign]

What is your post setting for this

arccheck : 1 #Check for small arcs, convert to linear

atol : .01 #Angularity tolerance for arccheck = 2

ltol : .002 #Length tolerance for arccheck = 1

Do you know that your backplot depends on your post file ?

 

Personally I trust my backplot more than verifier .

And same time saw a lot of times when one post file shows some issue on backplot and other one not.

I used with ver9 my post file ,changed chaining

tolerance and saw issues ,you may not see them

This reminds how I scrapped one part in Cimatron ,they have some setting like loops check global ,local and off .

It was off ,and tool made nice loop 360 degrees and scrapped the part .

I think it goes from the gap in the contour .

It was produced through model slice and may have microscopic gaps .

Now when chaining tolerance is greaater than gap your toolpath is tangent approximation .

MAy be it is not tangent enough .

A little intercrossing or gap produces same result in Contor offset ,I think irt is a problem of algorithm

Have a look

 

[ 06-01-2006, 05:33 AM: Message edited by: Iskander teh Owl ]

[DavidB]

quote:

---

What is your post setting for this

---

From my post..

code:

---

arccheck    : 1     #Check for small arcs, convert to linear

atol : .01 #Angularity tolerance for arccheck = 2

ltol : .002 #Length tolerance for arccheck = 1

---

[Josh_Petitt]

DavidB, did you ever find a definite solution to your problem. I am also seeing the tool gouges when I change from "Reverse Wear" to "Control".

[DavidB]

Josh,

I got aresponce from QC re garding 2D chamfering using comp in control

 

quote:

---

When you do this you’ll see that there is a problem with the offset algorithm and chamfer tools.

 

I can’t get it to cut the left most nose radius of your part.

 

I logged a bug against it. It is defect # CNC 00021413.

 

---