Randomly changing tool planes in 5 axis

[Bruce Caulley]

I have just had a problem with the tool planes on an existing 5 axis mastercam file. Some of the toolpaths have "reversed". The programmes that were originally posted are correct, but when I went to make some modifications some of the tools appear to be coming out of the table and not from the spindle. Internal profiling is now external profiling etc..... Not all operations are effected.

 

Bruce

[Mike Whitten CAD/CAM Contractors]

Are they both from the same version of Mastercam? If no, what are they from?

 

Are they actually "Multiaxis" operations or are they just Five axis positioning ops? If they are "Five axis positioning ops?", are they using named views or just having the TP/CP set?

 

Thanks,

 

Mike

[crazy^millman]

Aslo need to make sure they did not use WCS for some and I have seen where I am doing a part with say 1200 Cplanes and then open it up the next day and only have 350 or so. This can be avergrating and most times try leaving those open untill completely finish or have put a toolpath on that cplane to lock that place in use even if the numbers change from day to day. I would even think maybe going from 9.1 to 9.1 sp2 might give the results but since we never did repeats can not really tell you.

 

HTH

[Mike Whitten CAD/CAM Contractors]

Ooh yeah Ron, The WCS is how a lot of people make a mistake. I forgot about that one.

 

Thanks,

 

Mike

[gcode]

Every time you make an arc that is not on one of the 8 standard construction planes Mastercam makes a CP(view) for that arc.

If you been translating models around in space, you may have thousands of CP's, many of them unused by the end of the day. When you close the file and reopen it, MC cleans up the database. You can get the same results by running RAM-saver in the File menu.

 

Try a little experiment.

Draw an arc in Top view centered on the origin.

Go to the WCS View Manager and set the radio button to "All".

You'll see the 8 standard views.

Switch to front CP, rotate/copy the arc about the origin 3 times @120 dergees.

Now look in the View Manager

Mastercam has created 2 more system views to accomidate the new arcs. Delete the arcs and check the View Manager. The 2 new views are still there.

Run ram-saver. Now the views are gone because

the arcs are gone and they are no longer needed.

 

MC does this every time you open file as well.

That is why the quantity of views change and the

number assigned to views change when you close and open a file.

Mastercam purges the unneeded views and renumbers the ones that are left.

Bruce, I' going to guess that the reversing toolpaths are being driven by arcs. You can draw an arc on the Top plane and the bottom plane.

They look identical but if you use the arcs to drive a 5X drill path you get 180 degree different toolpaths. Analyze the arcs that are giving you trouble. I'll bet the view is 180 opposite what you expected it to be.

 

 

To help understand this, do the experiment again.

This time rotate 6 times at 60 degrees. The visual results look identical, but you now have 4 new views instead of 2. You would have a very hard time putting 5X drillpaths on this geomtery.

The exact same arc can exist on 2 different views,

180 degrees apart.

 

If both views are in the database, MC has a 50/50 chance of keeping the one you want when it purges the database. If you created the arcs from solid edge, it may be 180 degrees opposite the view you expect it to be

 

I use Drill 5X points/ lines for 5x drilling.

You get much better results once you get use to it.

[crazy^millman]

quote:

---

I use Drill 5X points/ lines for 5x drilling.

You get much better results once you get use to it.

---

This to me is one of the best ways to use this toolpath.

[Bruce Caulley]

Thanks,

It just happened again!!! I opened a job to get some sizes for our QC dept and ,lo and behold, more operations are upside down. These are 5 axis positioning ops and not 5 axis moves. The programmes as originally posted are fine but maybe moving from one seat to the next as sometimes happens in our office can bring about a conflict with some configs??? All seats are v9.1sp2

[Mike Whitten CAD/CAM Contractors]

BC10146,

 

Are you just changing the TP/CP or are they named views?

 

If you have no other options:

I believe that you may just have a wierd glitch and something is corrupt.

We do Five axis positioning all day long(named views) between two seats of software. 9.1sp2 and now mr0304. We have never had this issue. If this were me I would save all my stuff and re-install. There is something wrong, 9.1sp2 will not do this!

quote:

---

The programmes as originally posted are fine but maybe moving from one seat to the next as sometimes happens in our office can bring about a conflict with some configs??? All seats are v9.1sp2

---

Mike

[Bruce Caulley]

Thanks for that. We are doing a bit of a software upgrade shortly so I will see if re-installing everything works.

[Mike Whitten CAD/CAM Contractors]

Are you just changing the TP/CP or are they named views?

[Bruce Caulley]

They are named views. First example is just an angled face with a couple of tapped holes in it. Programmes verified, posted and ran perfectly. 2 weeks later I opened the file to check something and all tools using that named view were upside down, ie drilling from the bottom of the hole to the top, facing the inside surface etc

 

Bruce

[Mike Whitten CAD/CAM Contractors]

Wow! ?

[Bruce Caulley]

Wow is not exactly what I said, but it was close enough.........