Subsequent holes..

[Rekd™]

I have noticed when using WCS for odd-ball views, when you create arcs or points, you now have to type in the X and Y values EVEN IF THE LAST VALUE IN EITHER AXIS IS THE SAME.

 

For example, I created a custom WCS, rotating the part around the way I am machining it, and set a WCS using Copy current G-View.

 

When I'm typing in locations for my holes, I used to do;

1,-.25 Enter

2 Enter

,-.5 Enter

-1 Enter

 

Now, with the new WCS, when I type just an X value, the Y goes off into space instead of keeping the last value used...

 

Anyone else notice this?

 

'Rekd

[TonyK]

Rekd

I had the same prob. but instead of out in

space the Y location was on the edge of

the part.

[mayday]

ya Rekd,

its wacked out. I could'nt figure out what was goin on

when I first seen it. that and I'm still fighting my view dislpy

flipin my part wrong all the time

[mayday]

while on the subject,

have you figured out an easy way to rotate the xyplane after selecting a solid face for a new wcs. never fails I cant get xyz to be in the proper dir. (not enough options to pick from.) so I agian have to do a rotate of the face I just picked. Screw it I guess, when it comes to settin up 4+ index moves in the wsc. Im sticking with named views and fliping my geometry the way I want it before I start.

[Rekd™]

Couple suggestions here..

 

1) create a library of the views you use most, then import them.

 

2) rotate the g-view to the view you want to use, then use Create/Copy Current G-View. (this is my favorite for odd-ball views)

 

'Rekd

[iowajim62]

mayday,

check which line you pick first

horizontal line = x

vertical line = y

in that order

works for me okay that way

HTH

[mayday]

Thats kinda what I've been doing

just a pain sometimes. would be nice if I could pick a position for the origin,then ckick on the axis nome and swing it the way I want and name it,save it.

some things I run into is,

I set up lets say 4 index moves for opp1 on a horz.

now I want to use the same mc9 for opp2, but the part has to set on a different side and agian set up 4 index wcs agian. my gview starts to get confused,keeps jumping around on me, and no I'm not drinking (right now)

 

[ 08-29-2003, 01:14 PM: Message edited by: May^Day ]

[mayday]

this is taken from the mpmaster post. now to me decribing the setup for 4axis horz. is in direct conflict with the way the wcs is supposed to work. whats your opinion.

I have no problems with the wcs when prog. for a virtical 4 axis machine

 

 

#Milling toolpaths (4 axis)

#Layout:

# The term "Reference View" refers to the coordinate system associated

# with the Top view (Alt-F9, the upper gnomon of the three displayed).

# Create the part drawing with the axis of rotation about the axis

# of the "Reference View" according to the setting you entered for

# 'vmc' (vertical or horizontal) and 'rot_on_x' (machine relative

# axis of rotation).

# vmc = 1 (vertical machine) uses the top toolplane as the base machine

# view.

# vmc = 0 (horizontal machine) uses the front toolplane as the base machine

# view.

# Relative to the machine matrix -

# Rotation zero position is on the Z axis for rotation on X axis.

# Rotation zero position is on the Z axis for rotation on Y axis.

# Rotation zero position is on the X axis for rotation on Z axis.

# The machine view rotated about the selected axis as a "single axis

# rotation" are the only legal views for 4 axis milling. Rotation

# direction around the part is positive in the CCW direction when

# viewed from the plus direction of the rotating axis. Set the variable

# 'rot_ccw_pos' to indicate the signed direction. Always set the work

# origin at the center of rotation.

[Rekd™]

quote:

---

and no I'm not drinking (right now)

---

AHA!! We've found the problem!

 

 

'Rekd

[crazy^millman]

Hey Rekd and May^day do either of you use the Bounding Box? I started using it for the turning of models and have very good results doing it that way. I will use the point created in the center of Box as control for all models from there. I was wondering if you have turned the part to be the way you are machining why would you need to then turn the WCS also would the default top tool plane do it right any way if you had a vertical machine probaly a stupid question just thinking out loud is all.

 

CRazy Millman

 

PS i owe credit for the Bounding Box to my co-worker he is the one that use to use in other Cam program and wanted it for Mastercam. I had not used it till he open my eyes about what it can do.

 

PS^2 Hey did I ever tell you why I didnt like college it only took me 6 times to pass college english 101.

 

[ 08-29-2003, 01:43 PM: Message edited by: Millman^crazy ]

[mayday]

sorry Crazy, I cant type worth a cat poop either but what did you say??

quote:

---

I was wondering if you have thrun the part to be the way you are machining why would you need t othen turn the WCS also would the default top tool plane do it right any way

---

[crazy^millman]

Hey Rekd man you are vefy smart and good at this. I am going to ask anotehr stupid question so you have the construction view set to the number you have made the part view and do you have the z set to the height you want. I found when doing 5 axis stuff I would sometimes have up to 400 views for construction and if I was in the wrong one this would ahppen alot. Just sharing crazy thoughts is all.

 

Crazy Millman

 

Hey no problem May^Day cant get spell checker to work on this thing.

 

[ 08-29-2003, 01:48 PM: Message edited by: Millman^crazy ]

[Rekd™]

I've never done any 5 axis, mostly 4 axis indexing. I create a point at my origin for each view, always setting my Z0 for that view. (My post takes care of the clearance plane issues.) Now, when I do toolpaths, I select the WCS for that view, then select the T and C planes for it also, (which will default to say TOP, but still works, not sure why.) When I change WCS's, my T anc C planes always stay at top.

 

Do you check "Reset CPlane/TPlane when switching WCS"? in the WCS manager?

 

I'm still confused on this one; this is from the help, and I am more confused now than before I read this... :/

 

quote:

---

The Reset Cplane/Tplane when changing WCS check box is located in the bottom right corner of the View Manager. When selected, it changes both the Cplane (construction plane) and the Tplane (tool plane) to Top when you change the Work Coordinate System (WCS). When not selected, the Cplane and Tplane remain set to their views. However, by redefining the WCS, their current views have also been redefined because view definitions are always relative to the WCS.

 

For example, if you change the WCS and select this check box, the planes remain as they were set, although geometry you create after changing the WCS will be in a different plane than before (because planes and view are defined relative to the WCS). If you change the WCS and deselect this check box, both Cplane and Tplane will be set to Top (that is, the new WCS Top).

---

I am not sure if I'm doing it right, but it works well, and by god I spent enough time figuring this crap out that even if it IS the wrong way, I'm gonna keep using it cuz I 'worked' for it..

 

HTH

 

'Rekd

[crazy^millman]

Glad to know i am not the only one that think that about that. I feel the same way if I get it to work and it does what I want then who is to say it is wrong. I think we both do the 4 axis the same way then only difference is I never use WCS. I also decide where I am going to make the Center of my rotation. I copy the part to different layers naming each rotation angle. Turn off the other layers then rotate the part to the place where I am going to do the machining. I have Operations Default Default4th set to Clerances of 6.0 and use that to keep from having to always change them and then I touch off all my tools using the center of rotation as my z control and go from there. If I am doing something that requires contious rotation then I am using the mulitaxis toolpaths like Flow 5ax I have not figured the other ones out yet for 4th axis rotary tool paths. If i am way out in left feild then sorry.

 

I had to make a X break roll die about 4 years ago on a Mazak VTC with full 4th axis with no Cam program I sat down in Autocad and Flattend out all of the Geomentry then I created .001 angle division everywhere my tool met the profile of the Contour I then spent another 40 hours writing all the G code to make the Male and Female Roll dies work together. The only break I got in the whole job was that the Parts were symetrical around the diameter 4 times. When I got one right then I made sub calls to repeat it on every quardant. If you got Autocad I will send you the files and check it out. Real Crazy Pain in the A??SH?T but I got it done and it worked perfect.

 

Crazy millman

 

Is it me or does this sound like double talk

quote:

---

if you change the WCS and select this check box, the planes remain as they were set, although geometry you create after changing the WCS will be in a different plane than before (because planes and view are defined relative to the WCS). If you change the WCS and deselect this check box, both Cplane and Tplane will be set to Top (that is, the new WCS Top)

---

[Thad]

Rekd,

 

I wasn't aware of this "bug" or the fact that you could type in the locations like that either. Thanks for the info!

 

Thad

[Allan Brown]

In my opinion the WCS is good for 3-Axis only. You leave the part as is in Mastercam, and dance the WCS around to create new 'Top' toolplanes. Matching the WCS to your toolplane means the post won't output and change in the rotary axis or axes. This allows you to position the toolplane to simulate multiple setups on the machine. Each WCS simulates how the part is held on the machine for that op.

 

For 4 and 5-Axis machining, you can only use the WCS to set your Top / zeroed out rotary (A0/B0/C0) reference position. As soon as you set the WCS to match your toolplane, the post loses that ability to calculate angles because you are effectively back to the top. All rotary axes are worked out from the toolplane with respect to the WCS. The only application of the WCS for 4/5-Axis is for 'in car' / 'in plane' positioning of geometry, rather than moving your geometry to your datum and machining orientation. In this application, ever operation should use the same WCS value - it's just a reset of your Top. Even with that, there have been some bumps along the way - for Transform Rotate ops, the cplane selection tends to be back in world coordinates, not the WCS, which can be quite confusing.

 

[ 08-30-2003, 08:18 AM: Message edited by: Dave Thomson ]

[Trevor Bailey]

Have you guys downloaded the WCS Tutorial from Jay's site? I am pretty sure it is there. It may fill in soome blanks.

[Chris Rizzo]

Man, there's been days that I love the WCS, and days that I hate the F$%$#ing thing! Why can't it just work! I go through the tutorial and help menus periodically, and review issues with my dealer/instructor/friend. Guess I need to vent them here, too.

 

Ok, from previous WCS threads (and there are alot of them), some people do it rekd's way, of just swithing the wcs for each op. However I believe that each time you change the WCS, you get eight freshly defined views...and what happens is that the number of views will exponentially grow. 8x8x8x8x8x8x etc. This explains millman's issue:

quote:

---

sometimes have up to 400 views for construction

---

and also the help menu

quote:

---

However, by redefining the WCS, their current views have also been redefined because view definitions are always relative to the WCS.

---

Personally from what I've been instructed and what the tutorial says, is that ONE WCS change per file is all that's necessary and/or recommended...to prevent the propagation of views (8x8x8x8x8). But then again there seem to be quite a few users who just switch the WCS for each op., and have perfectly fine results; if anything a better time just making each machined face the "top"....please someone chime in if I'm wrong...I'm just reviewing the root of the WCS here.

quote:

---

never fails I cant get xyz to be in the proper dir. (not enough options to pick from.) so I agian have to do a rotate of the face I just picked

---

Yes, a big issue that drives me crazy sometimes. Sometimes I actually draw in my desired geometry as short, labeled lines on another level. x,y,z. Good reference when visiting old files too. I am glad they fixed the graphics issue related to this in 9.1, though. That has helped slightly. At least you know what your getting, versus a shot in the dark.

 

quote:

---

Even with that, there have been some bumps along the way - for Transform Rotate ops, the cplane selection tends to be back in world coordinates, not the WCS, which can be quite confusing.

---

YEAH, no kidding! I hav'nt done any transformations recently, but have had some very frustruating days doing many transformations in the past. I've know that there were problems with transforms, and just ended up working around them instead of wasting more time investigating and solving.

 

Ok, enough of the my Biblical WCS post...I'm earning my avatar the long way!

[crazy^millman]

Ok Dave going to quote you here to see if I understand you correctly.

quote:

---

For 4 and 5-Axis machining, you can only use the WCS to set your Top / zeroed out rotary (A0/B0/C0) reference position. As soon as you set the WCS to match your toolplane, the post loses that ability to calculate angles because you are effectively back to the top.

---

I now think that upon what you said that the way I do is the best for me using Mastercam, but more than willing to have soemone show me I am wrong.

 

I looked back through my old 5 axis programs. I did not have to pick a WCS for the different planes I was working in. I had the WCS set to the origin of the Part relative to where I called it on the machine. I then did all of My operations from there. I would have different T-planes and C-planes relaitve to the operations I was doing, but only used one WCS. It as very cool to set a 30 degree T-plane and then tell the head to machine a real tall face didnt have to stick your tools out as far to do that.

 

 

I said before I never use WCS and I am wrong I used it sometimes on 3 axis stuff to put the orign for programming the part in a different place verses moving the part. I know it may take a little more time but I will keep translating the parts to the origin. I think in reading this thread and others I finnaly get the WCS thing for 3 axis work and multi parts. I still think I am going to use the workoffsets in my operations. I can take one parts and using 10 different operation with 10 different workoffsets create 10 different parts. I understand that I could do it with the WCS. I have found for me in my simple brain that if I keep myself doing things the same way I keep from getting confused. I do 4 axis work as well as 3 axis work and hope to one day doing 5 axis work again. By the way love what Mastercam does in 5 axis it is awesome. If I start changing the way I program the 3 axis I put myself at risk to do 4 & 5 axis programming thing wrong.

 

Well that is my 10 cents worth today.

 

Crazy Millman

 

[ 08-30-2003, 12:04 PM: Message edited by: Millman^crazy ]

[Rick Damiani]

quote:

---

that and I'm still fighting my view dislpy flipin my part wrong all the time

---

Go to Screen|Config, select the 'Screen' tab and turn on 'Free Rotate'. It's right under 'Enable OpenGL'

 

Got that tip here, actualy.

[Chris Rizzo]

Ok, I'm on a mission... I just watched the WCS video from the FTP site, and re-read the WCS tutorial directly from CNC Software...and they contrary to one another.

 

- The video has the programmer changing the WCS for machining different sides of the part.

 

- The tutorial says:

quote:

---

One common misunderstanding is that anytime you need to work on different faces of the part or work on non-standard planes, you need to "use WCS". This is not correct-Mastercam already includes tools like Cplanes and Tplanes that let you do this. The ability to redefine the orientation of the WCS is a useful new tool; however, like any tool, it is only appropriate for specific applications.

---

What gives? I've uploaded the CNC provided tutorial on the ftp site here. If y'all don't have it already.

[Harryman]

To the extent that I understand the issue, a litmus test for WCS might be: If you will be fixturing to align the physical part with the machine's axis, use WCS. If you are using machine axis to align with part features, don't use WCS.

 

My $.02.

[Thad]

quote:

---

- The video has the programmer changing the WCS for machining different sides of the part.

---

cmr,

 

I haven't seen the video or gone thru the tutorial (yet), but that's exactly how we use the WCS and it works fantastic.

 

I never used different WCS before V9 and I hear people talking about the "old way" with T/C planes. Maybe the help file just needs to be updated???

 

Thad

[Rick Damiani]

Harryman is correct: use the WCS if and only if you will be moving the part to a new location to work on the other sides. For 4 and 5 axis work, you must rotate the tool plane or MasterCAM will not calculate the angles or make them avalable to the post.

 

cmr, this statemetn in the tutotial:

 

quote:

---

One common misunderstanding is that anytime you need to work on different faces of the part or work on non-standard planes, you need to "use WCS". This is not correct-Mastercam already includes tools like Cplanes and Tplanes that let you do this. The ability to redefine the orientation of the WCS is a useful new tool; however, like any tool, it is only appropriate for specific applications.

---

is explaining that using the WCS is not *required* when you are re-fixturing to work on other sides of the part. You could, if you wish, rotate or relocate the tool plane to achieve exactly the same results. In fact, that is how you would handle such situaitons prior to the WCS feature being added in V9. The WCS is a new feature that can make certan kinds of common tasks easier if you choose to use it.

[Chris Rizzo]

Ahhhhh, I can see that I might be interpreting that quote as:

 

- it is not correct to change the WCS for each part face.

 

when in fact that statement is saying:

 

- it is not necessary to change the WCS to machine different faces.

 

It seems that you can either:

 

A) Change the WCS for each side

 

or

 

Leave the WCS where it is, use different t/c planes for each side.

 

Both methods accomplish the same thing. However, if you both change the WCS multiple times and use various t planes in relation to each WCS shift, then you get all sorts of multiple view propagation...8 views each WCS change. Right? I'm assuming that's the reason I was taught NOT to keep changing the WCS for each face.

 

To summarize- To change faces, use one system or the other...but not both.

 

- I hope I'm not thinking too much about all this, but judging from past WCS threads, there is indeed valid confusion. Thanks for taking the time to help me get it.