I need a post....

[Nominal]

FIX!

 

I have a 4 axis post that was updated from version to version etc...

 

The error message I'm getting is..

quote:

---

Only single-axis rotation is allowed!

Angles may be incorrect.

---

The post works ok except when I try to cut things in view #3 (back side). I still get all the code except it skips the output of any rotary angle.

I get that error message for any operation done in view #3. The message seems to imply that I'd need a 5th axis to make the cut, which is totally false. The backview is confusing it somehow.

Any ideas?

[Guest CNC Apps Guy 1]

You're not using the WCS to define the back view are you???

[Nominal]

No James. I haven't changed the wcs only the tplane

[Roger Martin from CNC Software]

quote:

---

Only single-axis rotation is allowed!

Angles may be incorrect.

---

If you ever see this.

It is in your toolpath!

You have flipped more than one axis from one operation to the next (check your X axis directions, that is usually the problem). You don't need to be using WCS to make this mistake.

[Nominal]

quote:

---

You have flipped more than one axis from one operation to the next

---

I have 31 operations all around this part. Everything works fine. Backplot/verify looks perfect. The posted NC code is perfect except it's missing the rotary move in 2 places. Both places are when I'm cutting on the backside.

If I edit in the two missing moves by hand it works fine. I don't understand how I would have flipped more than one axis. All I did was choose the tplane, choose the path and cut. 31 times. Every other plane works except the backside.

 

quote:

---

You don't need to be using WCS to make this mistake.

---

What mistake, and how am I making it?

[mayday]

go to view 3 and create your C/T plane i.e. X,Y direction. in your toolpath T/P plane turn off wsc and select your created plane in the tool and constuction plane. When it comes to multi indexing I stay away from WCS. it can mix things up on you in a hurry.

[Lathe-Mill]

9/8/2003

SAME PROBLEM

here is the answer

quote:

---

The problem you are having is due to the tplane and cplane.  There is an odd thing that happens with our defined back plane.  What you have to do is to create a new tool plane that has the correct orientation when the back plane gets rotated up to the top view.  The easiest way is to go to the back plane, create a rectangle, and then create a tool plane from that rectangle.  Select a the upper long leg then the vertical right leg.  You may have to hit next a couple of times to get the Z pointing out towards you.  That is the orientation that will give you the correct rotation when brought to the top.  It is an ongoing problem in our software with the back plane.

 

 

 

Regards,

 

 

 

Tech Support

 

CNC Software, Inc.

---

I called my reseller, the did guide me and i was able to do it....i had also around 20 ops.

[Nominal]

Jim,Roger,Mayday

 

Thanks for your input.

 

Carlos,

 

Did I mention lately that you're the man!

Yeah thats exactly what it was. I suspected something was buggy about the back plane. I did what you suggested and it all works perfectly.

 

 

P.S. props to Mayday he also had the answer.

[Lathe-Mill]

you're welcome

[crazy^millman]

Yeah Thanks Carlos been having the same freaking problem finnaly went back to my old turing the model method makes for some edting but I know it works.

 

 

Crazy Millman

[heeler]

I have alway taken the top view and rotated the Y axis up 180 degs to cut the bottom of the part.

 

HTH

Glenn

[Roger Martin from CNC Software]

Yes, I've gone into great detail with this explanation. Maybe too much for experienced MC users.

The Post Dept gets the "My post is not working, I get the Single axis rotation error" a LOT.

So I'm not picking on you Nominal

 

This explanation assumes that you are indexing around a part on your VMC.

 

If you do not have a sample drawing, do this to make it easier to see.

 

Draw an 6"x4" rectangle in the Side Cplane centered at the Origin.

Set the Gview to Isometric (this just makes it easier to see what you are doing)

Xform-Translate (using Join method) that rectangle "-10" in the Z axis.

 

1>

Set the Tplane to TOP.

Press ALT-F9 to display the axes.

Looks like you would expect...

 

+X axis going to the "right"

+Y axis going "out thru the back of the part"

+Z axis coming "up" out thru the top of the part

 

 

2>

Now set the Tplane to '3'

Press ALT-F9 to display the axes.

Looks like you would expect... if imagine yourself looking down the Z at that face

 

+X axis going to the "right"

+Y axis going "out thru the back of the part"

+Z axis coming "up" out of the part

 

But wait!

When you index to that face (Tplane #3) into the real machining position on your VMC, which way the +X axis pointing?

 

On the machine the +X to the right - correct?

Refer to Step #2 above.

Look at the axes displayed in MC

Notice that in addition of your +Z being rotated (which you wanted), that the +X is pointing in the opposite direction!

 

That gets you the ->

quote:

---

Only single-axis rotation is allowed!

Angles may be incorrect.

---

Because you have rotated TWO axes going TOP or FRONT into that view. Note that if you just post operations that are in that view, the post will not complain. Everything was in that one view. The post will complain only when going from processing toolpaths in one view to an new view and more than one axis has changed directions.

 

Do you need to use WCS to 'fix' this? NO.

People forget that when you click 'WCS' on the menu, you are going into the VIEW Manager.

Use the Named View feature!

 

Go into the View Manager. (click on 'WCS')

Right click on the 'System View 2 - Front' and select 'Create' and then 'Select menu'

Select Rotate, Y+ up, and enter '180' for the rotation angle and click Save.

Your are now back on the View Manager dialog.

Enter a user friendly name for this view.

Now whenever you need to set Cplane or Tplane or Gview to the "back side", just click Tplane, Named and select that Named View.

[Nominal]

quote:

---

You have flipped more than one axis

---

Did "I" do it or did MC do it for me?

 

Thanks for the explaination Roger. Is there a long term fix for this, or is this the long term fix?

[crazy^millman]

Ok I undersatnd wht I have secuess soemtimes and not others I do the transform rotate so it keep x the same whre as I so the C-plane I do make the Axis swap so I do have to create C=plane which relate to the t-plane right or I have to grab the WCS to make it work wirhter way will work but still have to take in account the postion of x,y,z relative the the face ofthe part as how will be looked at ni the axis of rotation to the top machining or veritcal position.

 

 

Crazy Millman

[Jimmy Wakeford from Barefoot CNC]

You can alter post to keep this alarm form happening, you just have to add some code for outputing angles.

 

Jimmy

[Guest CNC Apps Guy 1]

I just have everything in the Top view, then use geometry to define which direction I'm going. Never fails.

 

Nice explanation Roger. Thanks. You'ere much more eloquent than I.

[crazy^millman]

James & Roger I was thinking the right way just not doing it the right way I finnally think I can say I got it. Where I didn't have problems with this when doing 5th axis work that would become problem when doing 4th axis work. Where as in 5th axis you can cover many sides of the part with one toolpath in 4th axis you are only really covering one side of the part at a time and the Mastercam program keep everything realtvie to what you tell it to. If you start on the top and then turn to the left you may turn to the left but you really also do some switching of your axis rotation relative to that original postion where as in 5 axis toolpaths the cover the whole part you may be doing work on the side but it all calcuated from the orginal start plane and thus keep all the calucation correct and going to the right plane and axises of rotation. This would realte to soemthing like a 5thaxisflow toolpath that woudl also not need many t-planes and c-planes where as a flowine on the right side of a part being done in a 4th axis would sound the same but worlds apart.

 

Crazy Millman hopes he see the light through all the fog in his mind.

 

[ 10-17-2003, 01:05 AM: Message edited by: Millman^Crazy ]