Hi Mick,
Attempting to address some of your Autocad issues......
"Autocad will only draw effectively in the top down view, you can't really draw in left/right/front or back."
This is absolutely untrue. You can draw with the exact same functionality, and for the most part with the exact same convenience, in any view in Autocad. This includes any of the standard 2d views like top, front, right, bottom, as well as any 3d view in any orientation. In fact, I probably spend 95+% of my time drawing in views other than the top view. It's fairly essential to seeing things clearly, and manipulating the model in all three dimensions accurately. The reality is that utilizing any given view has very little to do with functionality of Autocad.
The real issue is the orientation of the User Coordinate System. Manipulating the ucs, and especially the z axis, is critical to drawing any kind of circular 2d geometry or curve-based 3d object in any orientation, top down or otherwise. The orientation of the z axis also has a direct impact on the behavior and results of a host of other commands and functions in Autocad, including but not necessarily limited to the Circle, Arc, Rectangle, Mirror, Rotate, Sweep, Offset, Extend, and Trim commands. It also affects the functionality of some object snaps like Tangent and Quadrant that deal specifically with circles and arcs.
In your particular work flow, it's important to remember that circles and arcs are always drawn in the xy plane. In order to draw your roof profiles from the side, you must first change the ucs so that the xy plane is vertical and coplanar to your desired profiles, with the z axis then horizontal and perpendicular to your profiles by default. There are a multitude of ways to change the ucs, but for your purposes I'll suggest three.
From the command line: ucs-->type your chosen orientation of top, right, front, and so on-->enter.
From the toolbar: Home tab-->Coordinates-->drop down menu-->pick your orientation.
From the toolbar: Home tab-->Coordinates-->Z axis vector (the icon with the Z in the top right corner)-->pick an origin point and another point on the Z axis. In this case, it doesn't matter where the origin point is, but rather which way the z axis points (unless you're entering absolute coordinates for some reason, then the origin point matters).
I'm a short key alias keystroke kind of guy that abhors using toolbars (too slow!!!
) so I would use the first option if I wanted a specific 2d orientation. When I'm in 3d, I usually use the Z axis vector method unless I need to worry about all three axes, in which case I use the 3-point method. But for circles and rotation (all rotation occurs about the z axis), I'm only really worried about the z axis.
The important distinction to remember about using the standard named ucs orientations versus the World ucs or a custom orientation is that in any standard named ucs, any point you pick defaults to the xy plane, with a z axis value of 0. In 3d ucs orientations, selected points can be just about anywhere in the infinity of the 3d realm despite where they may appear to be, unless you specify coordinates explicitly, or snap to existing points.
Another thing to know is that if you select a named 2d view from Home-->View-->3d Navigation pull down menu, the ucs will automatically be reoriented to match the view. Selecting a 3d isometric view from the same menu
will not simultaneously change the ucs. Also, changing the ucs to a named orientation
will not change the current view.
And lastly for now, even though not specific to this work flow, the ucs orientation is part of the information saved when you create a block or copy entities to the clipboard. When pasting or inserting, Autocad will reorient an entity so that it's saved ucs matches the current ucs, so objects may end up rotated, backwards, or upside down from what you might intend. This can be resolved by rotating things back to where you intended, but it is simpler and more robust to keep an eye on the ucs from the beginning. In the same vein, I like to set the ucs back to World when I save finished models, especially as I often xref individual parts into more complex assemblies, which often get nested into even larger assemblies.
Moving onward (finally...
)
"...and they must, must oh must touch at the vertices (points at each joint) on the flat parts, if they are out by one millionth of an atom then the part will not loft, form or join together..."
I presume you are saying that the profile must be a closed loop in order to create a solid from it, which would be correct. Much like you can't create an .stl without a watertight mesh, you can't create a solid from an open ended profile. You can still loft the profile, but you'll end up with a lofted surface instead of a solid. This is still useful in plenty of instances, but not this one. Hopefully you are using object snaps to ensure that endpoints of lines meet, or cleaning things up with fillets or by trimming or extending. I'm a big fan of object snaps - snaps equal precision, which is important to me, and they also equal convenience, which is equally important.
"Again select each outline in sequence and join together to form that block, and here in lies one of Autocads foibles. Each of the roof sections is a stand alone section, so each one has the same properties, however the forehead ones are all joined at their base and rotate around that base line to give a smooth arc. As far as Autocad is concerned it will now only join sections whose base is attached to another section, it will not join sections that are free standing along the roof."
I'm not 100% sure I am fully understanding this comment. But I think you are saying that once you form the forehead profiles into a solid, you can't them loft that together with the roof profiles. If so, then that would be correct as far as I understand. But what I would have probably done is copied the last forehead profile, the vertical one where it meets the roof, so that I had one copy to create the forehead and a second copy to loft together with the roof profiles. If everything behaved properly and as hoped, the result would be two solids sharing the same profile where the roof and forehead meet. Now of course the loft command can be a fickle mistress, often yielding unexpected results. It doesn't help that I don't always understand all of it's capabilities and processes fully, nor do I have a full grasp on some of the math behind it. I only just really learned of the idea of guides or rails when somebody mentioned it in a Rhino work flow in that recent smoke stack thread. So this may not work at all, or it may work but produce an unsuitable result. Only experimentation will tell.
"The headlight cone is an off set cone and once again we run into Autocads inflexibility. If I were to make a cube and select the top surface I can move or transform that in anyway I like and the resultant sides will adjust accordingly, however, as soon as there's a curve in it then the only function you can do is pull the top face up and down, you can't move it left or right, front or back, making it impossible to make an offset cone from a parallel cone."
Actually, creating
and editing an offset cone is pretty simple. The trick is to manipulate the cone as a surface rather than as a solid,and then convert it to a solid once it's the correct shape.
For whatever reason, Autocad restricts editing of solids formed from curved geometry to essentially only allow extrusion, whereas rectilinear solids enjoy almost unlimited freedom to manipulate edges and faces in any way seen fit. But Autocad does allow manipulation of surfaces formed from lofting curved geometry. I have no idea why one works and the other doesn't, but I don't really care
. I just chalk it up as one of those things. Because the lofted surface maintains a parametric association with the original geometry, manipulating the original geometry dynamically manipulates the associated surface. You can disassoicate the geometry and the surface if you like or need to, but that won't suit our purposes for this work flow.
Start by drawing the two circles you will use for the top and bottom of the cone, one above the other at an appropriate distance. You can go ahead and offset one circle now if you like, or you can do that after lofting. The two circles can even be the same size, as you can scale them as needed to get the appropriate height and taper for the desired cone.
Use the loft command and the two circles to form a truncated cone. Autocad defaults to creating a 3d solid, but it can be forced to create a surface instead. After initiating the Loft command and picking the two circles, choose MOde in the command line immediately after selecting the two circles, and before hitting enter. You will get the option to choose SOlid or SUrface. Choosing SUrface will force Autocad to create a lofted surface. Using the gizmo, move one circle sideways to create the desired offset if you didn't already position them before lofting. Then either move the circle up or down to change the height (and therefor angle) of the cone, or switch to the scale gizmo and adjust the the circle's diameter. Scaling would be appropriate if the height of the truncated cone was already correctly established but you still wanted to edit it's angle.
Once the cone is of the desired shape, convert the two end circles to regions using the Region command. A region is simply a 3d solid with no thickness. This is a necessary step before converting the surface into a 3d solid. Note that you must have a closed loop to create a region, and you cannot have overlapping lines. All segments must meet at a single point, which is of course moot when dealing with a circle. But this goes back to the closed profile discussion above. In fact, converting to a region is a good method to test the integrity of profiles before attempting to loft them.
In an obliquely related note, I prefer to use the Region command rather than the join command to form a group of lines and curves into a closed profile. Often when curves are involved, the Join command will output a spline instead of a polyline. Splines cannot be exploded after they are created, and they behave oddly with respect to object snaps because the points that define them are often not where you'd expect them to be. For example, you can draw a spline that looks exactly the same as a circle, but you can't snap to it's center or quadrant points. Conversely, a region can be exploded and it's parts revert to their original forms, and object snaps behave exactly as they should. The join/spline issue doesn't happen all the time, and really never when joining only straight line segments, but it's often simpler to just use the Region command instead. Splines BAD
!!! Hulk hate splines
!
Getting close now, finish up by converting the two circular regions and the lofted surface into a 3d solid using the Surfsculpt command. Select all three entities and hit enter. Presuming all parts combine to form a watertight volume, the result will be a 3d solid. Remember that the 3d solid will now be subject to the same infuriating editing constraints as before. So it's a good idea to save a copy of the original geometry and surface before converting to the solid form, in case you decide something needs to change again. Like that ever happens
. It's always a good practice to save a copy of your geometry.
That's it for now. I should probably go to bed. I'm probably a day or two late as you seem to have solved many of these issues already, but maybe this information can help in some way going forward. I've downloaded the FlashBack recording software. Tomorrow I will get the microphone going. So if you have any further questions, or need a video demonstration to make things clear, I should be able to create something in the next day or two.
Cheers!
Jim