tool plane

[Accu-Molder]

When changing my toolpath coordinate (toolplane ) in version X it updates all of my ops. How can I get this to change each operation seperately like in version 9.

[brilu397]

I ran into this about a week ago and I ended up making a new wcs for each coordinate using the wcs manager.

[Accu-Molder]

does anyone know if this is a bug. or has anyone sent it to cnc software if it is.

[Storkman]

On the first page of the toolpath parameters is a plane button. Select it and expand, you can change WCS, cplane and tplane for each operation.

[Accu-Molder]

This is were I changed the toolplane but it updates all operations not just the active operation. So if I have 10 operations and update the 10th one the first 9 operations also change to that number.

[brilu397]

Same happened to me.

[Doug Nemeth CNC Software Sales]

Are you changing the t-plane or just the work origin or both? I just want to make sure I'm understanding the issue.

[Accu-Molder]

Want to change toolplane only but when I select a point it updates,working coordinate system,comp/const. plane. In 9 you could set toolplane independently is this not the case in X.

[Doug Nemeth CNC Software Sales]

I can't seem to repeat this issue. I can have different tool planes and origins for different operations, and one does not affect another.

 

If I change my t-plane and/or work origin for one of my operations, it only affects that one.

 

I am running a production candidate or MR1, so maybe this was a bug that's now fixed.

 

Accu if you'd like to e-mail the file to me, I'll take a look at it.

[Accu-Molder]

Doug,check your mail.

[crazy^millman]

I think I might know where this might be confusing. If you pick the plane at the bottom of X you need to ignore that (WCS) that show next to planes. and Gview. That (WCS) has not a damn thing to do with WCS in my humble opinion though I have been told I am crazy whats new there). I as in V9 pick my c-plane before doing any toolpath but if you need ot do a toolpath or are doing a toolpath and want ot change plane it takes a little work. You go to the views like you think but you need to expand that to the tool-plane pick the view then it will give you the c-plane yeah weird to go thouh all the steps to do what was standard in V9. Again the biggest reason I make sure I am in the c-plane before starting any toolpath in X. I do like the fact we can name that view if not the standard view unlike in V9 where you had to copy the view to name it.

 

I think you are unknowingly using the WCS not c-plane and this is causing you the problems you are seeing. Me perosnally I only use WCS for 3 axis work for 4th and 5 axis work I still only want to use C-planes(goes against what most want but it gets the job done and keep my simple brain in tact).

[Doug Nemeth CNC Software Sales]

Thanks for the file Justin. I believe that the problem is that in X, we've done away with numbered and corresponding system views. Let me explain:

 

In V9, when you created a new origin, Mastercam would create a new system view, although most people didn't know this because it happened behind the scenes. So if you had 5 origins all in the Top view, there would actually be 5 different system views for each. This is why if you changed one, the others would not be affected.

 

In X, we did away with system views and numbered views for a lot of reasons, most to do with simplification. What this means is that all origins created in 1 plane will be linked. The solution is to do what Brilu said: create a new named view (multiple copies of TOP for instance)for each origin that you want. You only need to do this for multiple ops with different origins that share the same plane.

 

I can see where this would be a pain and create extra work, so we're going to look at this and see if we can do something to make it work more like V9 while at the same time not reintroducing system and numbered views.

[Accu-Molder]

I stay in the top c-plane but only want the tool origin changed for different locations of electrodes in a cavity wich it changes but updates all of the operations not just the one I want.

[Accu-Molder]

This will be a pain in the a$$ if I have to create a new named view for each different toolplane that I need. I use 10 to 50 different toolplanes in the same file in ver 9 with one step selecting the point. I don't understand why you would want them linked.

[Guest]

Justin,

 

Do all of your planes use the same origin?

 

I have found that when doing work on different planes that you need to zero out your reference positions on the created planes so the they maintain their relationship to the actual work zero origin.

 

I don't know if this is the problem you are having or not.

[Doug Nemeth CNC Software Sales]

John-

 

His problem is trying to use multiple origins in the same plane.

 

Try creating 2 random circles all in the Top plane. When toolpathing the 1st one, use it's center as a new origin (through the Planes dislog). Now do the second arc and set the origin to the center of it. You'll notice that it will corrupt the previous operation, because you're actually moving the origin for it too. I think this is the problem.

 

The workaround is to create multiple named views; 1 for each origin. It's more work than before and I've already logged it.

[Accu-Molder]

What we're doing is say you have A 2" square block with a .050" c'bore on the block @ x.250 Y.25 my world coordinate is the center of the block but I want the tool plane origin @ x.250 Y.250 so that when I cut the .050" boss I can use a 1/8" round stock and my machine cuts it on center becuase the toolplane is centered over the c'bore. This is just a simplified example of what I'm doing. I'm not sure if I'm confusing everyone more or if were all on the same page. All try to get a good example and cut and past it in here.

[Accu-Molder]

Yes, what Doug said I hope there is an easy way to change this in X.

[Accu-Molder]

Well. I cant get a snap shot of the screen on here. Do I need it linked to photobucket or something? I was trying to cut and paste.

[Guest]

yeah , photo bucket will do the hosting, then from full reply form click image and paste in the url of the pic location.

 

I did recreate it, darndest thing too, never noticed that B4.