Mc9 Wire Post

[Rob G]

I have recently upgraded from Wire Mc7 to Mc9.

I am having problems with posting from Mc9.

Eg1. If I program a round hole with the start point being the origin one of the first commands in my post is G92 X0,Y0.

 

Eg2. If I program a round hole with the start point being X5.00,Y0 the first command becomes G92 X5.00,Y0.

 

However because my machines dont have automatic wire feed I am manually pitching between appatures. Therefore would prefer the values to be X0,Y0.

 

Is this a mastercam function that I can select wilst programming or a posting problem.

 

I thank those in advance of any sort of feed back they can provide, it will be greatly appreciated.

[Thad]

Welcome to the board.

 

I can't help you out except to say that it's a post issue. Possibly has to do with your misc values. If you open your PST file with a text editor, you should find pretty easily where/how MC establishes your pickup point (G54, G92, etc). Good luck.

 

Thad

[CAM-mando]

Try playing with the STCW values.

 

Also try placing a point at your thread position then when toolpathing chain the point then your contour in the same operation.

 

Also are you running 9.1 or 9.0. There were a number of changes to how MC handles cut and thread points in 9.1.

[Thad]

After re-reading your post, perhaps I misunderstood you.

 

Thad

[Roger Martin from CNC Software]

quote:

---

I have recently upgraded from Wire Mc7 to Mc9.

I am having problems with posting from Mc9.

---

Are you using a different Post Processor now in v9? or did you update your v7 post using the UpDate Post commnand in v9 ?

 

If you Updated your existing PST, I would assume the problem is how you are programming in MC.

 

And are you running Wire v9.0 or v9.1?

How the Start/Thread/Cut positions are programmed is different between 9.0 & 9.1

Ultimately the SAME data gets to the post in either case, this is really just a change the the programming method to define and select the Start/Thread/Cut positions.

 

quote:

---

Is this a mastercam function that I can select wilst programming or a posting problem.

---

Depends...

Usually (this is post dependant) you will get a 'G92XY' at the Thread Position. So if you are programming a dowel hole that is drawn with it's center at X5, Y1 and that is your Thread Point position, I would expect to get a "G92 X5 Y1" block output.

 

There are MANY user preferences concerning the code sequence to output at the very start of a Wire program and what to do after positioning from a cutout to another. That is where the post comes into the picture.

 

1> At the start of a program...

You can have the Start position different than the Thread position.

Say the Start Pt. is set at X0,Y0 and the Thread Pt. is at X5, Y1

 

Some users want this ->

G92 X0 Y0 (Start Pt.)

G00 X5 Y1 (Rapid to Thread Pt.)

G92 X5 Y1 (Re-G92 at Thread Pt.)

G01 G41/G42 X Y (lead-in to contour)

 

Some users want this ->

G00 X5 Y1 (Rapid to Thread Pt.)

G92 X5 Y1 (G92 at Thread Pt.)

G01 G41/G42 X Y (lead-in to contour)

 

Some users want this ->

G92 X5 Y1 (G92 at Thread Pt.)

G01 G41/G42 X Y (lead-in to contour)

 

Depends on machine setup technique, auto/manual wire thread, personal preference, etc...

 

2> At the start of a program...

You can have the Start position set to the same coordinates as the Thread position.

Say both are at X5, Y1 in this case.

 

Some users want this ->

G00 X5 Y1 (Rapid to Thread Pt.)

G92 X5 Y1 (G92 at Thread Pt.)

G01 G41/G42 X Y (lead-in to contour)

 

Some users want this ->

G92 X5 Y1 (G92 at Thread Pt.)

G01 G41/G42 X Y (lead-in to contour)

 

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

 

Now you have what to do when moving from one cutout to another.

Say that the Thread Pt. position of the 2nd cutout is at X4, Y2

 

Some users want to re-G92 at the new Thread Pt. position and some do not ->

 

G01 G40 X Y (lead-out of cutout #1)

"Cut wire" (Manual 'M00', Auto 'M21', 'M12', etc)

G00 X4 Y2 (move to Thread Pt of new cutout)

"Thread wire" (Manual 'M00', Auto 'M20', 'M6', etc)

G92 X4 Y2 (DO THIS AT THE NEW THREAD PT.?)

G01 G41/G42 X Y (lead-in to cutout #2 contour)

[Rob G]

Thankyou very much Thad for such a quick reply. I will look into all the information you've provided and see if I can come up with a solution.

 

Due to our company being so busy it's not often that I get a chance to sort out problems like these. At times it just becomes easier to program through Mc7.1.

 

However would like to get to the bottom of this for my own benefit more than anything.

 

Thanks again I am very appreciative.

 

P.S It is Version Mc9.1 that I have.

 

Regards

 

Rob Grose.