Iso vs. Ortho vs. Perspective take 2

[Mike S @ S4A]

I noticed a thread got started today on this topic which frankly had some inaccurate information in it. So to set the record straight:

 

Isometric - refers to a point of view (POV)

rotated 315 degrees from top and 45 degrees from front. From this POV multiple flat planes are visible. Also a valid construction plane in Mastercam.

 

Orthographic - basically means flat. in AutoCAD switching from 3D construction to ortho is like switching from 3D to 2D construction in Mastercam - you're restricted to drawing in one flat plane at a specific elevation. So you could draw ortho (2D) on any valid mcam plane.

 

Perspective - Has no use in CADCAM geometry or toolpath construction. It simulates for rendering purposes the "vanishing point" effect.

One guy made a good analogy; hold a cylinder up to your face - the end closest looks big, the far end looks small. Very effective in illustrations or renderings but if you were cutting the cylinder you wouldn't want to make one end smaller than the other right?

 

We expend a lot of energy in Training and Tech Support to keep our guys squared away on planes, views, and the WCS. I think part of the problem may be the use of the word "view"...

 

To quote directly from the S4A curriculum:

 

Obviously the use of the word “View” in multiple contexts like this can be both ambiguous and confusing.

By contrast the word “fire” in Naval Aviation refers only to the discharge of a weapon.

The presence of smoke and flames is referred to as a “conflagration”.

 

Our goal at S4A is to make absolutely clear explicit meanings in specific contexts. So when a particular coordinate set is used to define:

• A Gview

it merely establishes our “human’s eye” point of view on model space. It has no bearing on how geometry will be constructed or how tools will vector in to cut. Also keep in mind that we move, not the part. Our point of view moves relative to the model in space when changing or rotating gviews. Think like Galileo or Copernicus; the sun doesn’t revolve

around the earth, right?

• A Cplane

only affects geometry creation. Not viewing or toolpath vectoring.

• A Tplane

affects only tool vectors.

 

One view will be called upon to serve an additional function and be identified as the WCS. In the Mastercam parlance the WCS is the Working Coordinate System.

 

Working Coordinate sounds a lot like Work Offset.

 

This is not the intended concept.

 

The view activated as the WCS determines the Global alignment of Mastercam’s 3D environment. All other existing views/planes will function relative to this global view.

 

Apologies to anyone offended by the blunt offerings here.

[Guest CNC Apps Guy 1]

A healthy portion of problems in machine shops is related to terminology. I don't see why CAD/CAM should be any different.

 

j/k

 

Very good explanation Mike.

[Mike S @ S4A]

Thanx CNC. The Navair analogies have been working well for me....

[Superman]

Mike,

Based on your thread,

I understand the use of WCS and T-plane, but, please explain why toolpaths require a constuction plane ( my geometry is created, WCS for my setup, T-plane for tool vectoring, but...??)

The only reason I come up with is that the operation uses this for internal calculations eg slices, stepovers, offsets etc.

[Colin Gilchrist]

Superman,

 

You are correct in your thinking. The construction plane is used for the slicing/intersection/offsetting routines.

 

An example I like to use is a right angle head with a wheel cutter. You would have Top for your Tplane, but might use Front for your Cplane and a Surface Finish Contour toolpath.

 

So the "Slicing" plane would be normal to the Z axis of the Front Cplane, but Mastercam would output the NCI code relative to the Top Tplane (with the correct matrix shift if you define your head properly).

 

This is naturally very difficult to understand, especially when you try it for the first time.

 

Cheers,

[Mike S @ S4A]

Sorry for the gap, was in training class.

Thanx for stepping in Colin..one final thought -

you'll note that in the planes settings of an op the C plane is explicitly identified as the

"comp/construction plane" not just construction plane. As a "construction" plane it functions only for geometry creation. as a comp plane it comes into play as Colin said - most of the time T & C planes will be the same...only advanced applications (aggregate/right angle heads, mill/turn, multi-axis) may need them different...

[Superman]

Thanks Guys

Opens up a whole new world.

 

So on a steep ( near vertical ) surface, WCS=TOP, T&C-plane=TOP would require a fine stepover, but, C-plane=FRONT would act as Z-level machining ( in a sense )??

( just thinking of options to move 4/5 axis work back onto 3 axis )

[Colin Gilchrist]

Most of the time you can pick a different toolpath like Surface Finish Contour to machine a vertical surface like you are describing, but technically yes. You could potentially have your comp plane set to Front and your Tplane set to Top with a parallel style toolpath for better stepover control.