New To CAD? No, but....

I've never moved anything using coordinates. It's the CAD equivalent of measuring off a print and hoping that everything works out OK.

Your 'hard to manipulate reference points' are what the computer provides to save you the calculations. A differential would have the reference point(Fusion calls them joint origins, and they can be vertices, edges, faces, hole centres, additional points or any other feature) where the centres of the pinion and ring gears meet. Or the pinion flange. Maybe one of the halfshaft flanges if you're weird. You would then use a relevant joint type to place that to your axle centre line. The joint function also allows you to offset it in any of the three main axes, and/or rotate it around them. So you could initially set the pinion angle, and skew the axle across the frame if you were modelling a Renault. And alter either angle when something else changed.

All these programs will display grids on planes, and the main axes. They also allow you to turn them off which is preferable.

Don't get hung up on 'Sketch'! Although TurboCAD seem to have built 3D on top of a full-function 2D drawing tool, in effect you are doing Sketches, which are a type of 2D drawing designed for making 3D objects, with 2D functions stripped out and others added. I suspect TC's 2D editor has led Nigel into the mire by mixing 2D & 3D functionality.

Coordinates are best used sparingly. Real wagons are built from connected parts, each fixed in some way to another. Ditto 3D CAD: models shouldn't be a shower of independent bits made to look OK by flying in close formation! Coordinates are simple at first, but cause big problems later.

Rectangle/circle positioning is solved in SE by drawing construction lines just as in 2D. FreeCAD is the same and I expect the others work that way too.

Sweep exists to solve bent girder type problems. They make a solid by running a profile along a 'rail'. Example is FreeCAD, but F360 and SE are similar.

1. Sketch the U beam profile on the XZ plane:

2. Open another Sketch on the XY Plane, and draw the length and sweep of the U-Beam:

3. Select both sketches and click the Sweep button, yellow & red centre.

All being well, the U-Beam will appear:

Not bad, but wrong - the sweep line is incomplete! No problem, looking at the History I see I've created a 'Body' consisting of an 'AdditivePipe' based on two sketches. One sketch contains the profile, the other is the sweep line. Within reason I can change both.

The missing line is added to Sketch001:

Closing the sketch redraws the sweep:

No dimensions yet- it's all been done by eye, correct shape, but not size. Generally best to add dimensions and other constraints as soon as they're known, but they can be deferred whilst the design is fluid. However, the model isn't finished until constraints have been added, and missing them can cause trouble. A later change might cause unexpected movement. Planned moves are wonderful, unplanned moves are annoying.

Best practice to give sketches and parts meaningful names in the history rather than the defaults:

In FreeCAD everything depends on what was done before; history. It can cause bother if an early step is adrift. SE's Ordered mode is also history based, but it also has a 'Synchronous' mode, allowing models to change irrespective of the history. Speeds development up, but can cause confusion. Then Ordered Mode is better. Solid Edge recommend learning Ordered mode first.

2D drawings are generated last from 3D models. Third/first angle are tick-box choices, the hard part is deciding what to dimension and caption etc, which is done with the mouse. Sections are easy. FreeCAD, SE, and Fusion are similar.

'Once I realised ... it worked fine.' sums up my learning experience. Nigel rejects the idea he has a 2D mindset, but I recognise the symptoms: I had it too! Perhaps the hardest part of learning 3D-CAD was unlearning a mass of earlier 2D ideas. 2D brings a blizzard of unhelpful preconceptions about how 3D should work. Nope! The operator has to adapt!

Dave

I think we've hit a snag: radially different CAD packages!

I have not given up entirely on trying to learn 3D CAD but the gaps between my attempts are becoming longer.

Everyone else here is using programmes other than TurboCAD, and those do the same things in very different ways! So I am reading here how others use methods not existing in TurboCAD, to draw the same things. Let's look at what I mean...

TC gives several options for creating plane figures and "solids" _ but the solid figures are in more than one form, with peculiar properties, and this is partly why it is so hard.

TurboCAD floats the image and plane-indicators against a grid (options include inch/metric and non-display). The 3D default view looks obliquely down at the grid: isometric, as the view-angle tool says. You can of course rotate objects to any angle in any plane.

This allows aligning major centre-lines or outlines to the origin, axes and grid; and placing objects by Snaps and/or co-ordinates and direct dimensions. So if I place an object at typed-in (1, 1, 1) from the origin or some other point, I know its Reference-Point will be (1.000000000, ditto, ditto) from that datum. If I then use the Copy tool appropriately, I know its offspring's RP will be at typed-in (x, y, z) translation or Aº rotation from its parent, again at n.0000000... accuracy. (You can also set you own co-ordinate origin, and definite angle or count-round increments.)

The RP in TurboCAD is the centre of the object's plane or spatial occupation: the dead-centre of a cube or sphere, on the centre of the long axis of a cylinder or prism. For an object not fully symmetrical, such as my chassis rails, it lies outside the object itself.

Using this RP correctly can be vital for 3D assembling parts other than by handy Snap points like vertices and edge-midpoints, but I find this very difficult. Luckily TC is flexible: allowing Assemble Part B to A by Vertex Snap, Move B across A by dimension-entry change, as accurately as above.

My error is not in using numerical values. TurboCAD expects numerical entries where necessary as it often is of course. Entering numbers allows for example, fitting parts along a shaft or across blank facets (surfaces); but I am using them where I need not, or should not. .

By trying to do the computer's work for it, a drawing that may look right by eye can hold tiny value errors preventing other editing tools from working at all. It took me a long time to learn that in drawing a plane figure from scratch rather than editing a "primitive" or by the Polygon-tool, I need Snap the lines together so the polygon can be filled (e.g. coloured, or cross-section hatched), copied, moved, extruded, etc. If one corner fails even invisibly, the extrusion is a wall of display-line thickness, not a solid.

To draw those bunker walls, I copied-in-place the outline to a very slightly smaller size - tricky on a non-rectangle and with a quadrant corner - and extruded both. The line thickness filled the gap. I see now I should really have extruded a Poly-line with one wall fractionally shortened to stop the figure closing. For its companion, I used mirror-copy or rotated a straight copy 180º. These are the only ways available in TC.

Incidentally, Nicholas, no half-shafts and gear geometry here. This wagon's axle is of traction-engine type, with the differential on through- and cannon- shafts; necessitated by using chain-drive.

The diff itself is a modified, ex- front-wheel-drive car unit, with a motorcycle sprocket on the crown-wheel's place. Consequently the datum-plane is that of the chain centre-line; not among the gears. The correct form is of the differential one the wheel, also traction-engine pattern; but I made the axle so many years before finding a photograph that shows this detail that it can damn' well stay like it!

.

I may try 3D modelling again, after a long break. For I need re-design the cylinders - machined from stock bar - as I made basic mistakes that some 20 years after I bored them, are now causing all sorts of unforeseen problems like studs penetrating steam-passages, and nowhere sensible for the valve-chest steam inlets!

TurboCAD is dreadfully poor compared to more modern offerings

Did you check out the two videos I made on the previous page, of how straightforward 3d CAD (MoI) can be?

I did your bunkers and your chassis in about seven or eight minutes - only approximations of sizes, but just to show the principle.

.

Martin..

Edited By blowlamp on 09/05/2022 12:34:59

To answer Dave (SOD....)

Looking at your version of those cranked channels....

Yes, a very different package but the idea that TurboCAD might have made its 3D mode an extension (extrusion?) of its 2D had never occurred to me. Though I am worried how to use it, not how it was written.

I could have extruded the basic section from a "polyline" rather as I think you have - perhaps did, I forget now - and I am not sure that this shows much difference in difficulty and work between the two systems. If I could have used TurboCAD more efficiently that's by me, not its designers.

To make that channel section in TC there are two or three alternatives, all probably of similar effort. I did not try going the whole hog with root radii and tapered flanges!

+++

How did I bend the steel itself? It is 50 X 25 X 25mm HRS channel, the nearest to what appears on the ancient photos that are my only source material; but probably of over-scale thickness.

I have access to a manual bender really intended for forming narrow-gauge track rails, and used that to chalk-lines and wooden straight-edge on a concrete workshop floor, finally measuring the rails back-to-back, by steel rule to ensure parallelism more importantly than absolute displacement I can adjust for. I doubt the originals were much more sophisticated!

The I-beam front axle consists of 2 lengths of folded 2mm thick sheet-steel channel welded back-to-back, dressed flush and cut to width. The channel was second-hand from I know not what, but very close to scale by the photos. (And I must have been better at welding than I am now!)

I think there might be a flaw in your attempts to draw in 3D. I recently commented on a youtube video where an A7 enthusiast is building an A7 replica racing car. I asked what CAD package he was using, it looked so bad at 3D I couldn't believe it was meant to do 3D. It was Turbocad. He slaged it off with a very choice swear word and finished by saying he was too old to try anything else. I was 65 when I started to use FreeCAD, and like A7 man, I found TC to be the biggest load of wossname I ever tried. Sling it over the nearest hedge and set yourself the task of learning Solid Edge or FreeCAD or MOI or use a crayon and draw on a piece of slate. just don't try to use TC.

Turbocad is the present you give to someone you hate.

Someone above mentioned how intolerant 3D programs are to the slightest imperfection in a 2D sketch.

This use to stump me in the beginning, and I forgot how big a problem it use to be for me.

If you are not snapping exactly to the endpoints of lines and such, then you can have tiny imperceptible gaps that can be difficult to track down and eliminate.

One way to avoid the gap problem is to over-draw every line, ie: draw the lines longer than they need to be, and then use the trim command to cut them off, thus ensuring none of the dreaded gaps.

Sometimes the trim command itself creates a problem, such as at the intersection of two curved lines.  The trim command can produce a small section of arc on top of another line; and this stops a 3D program in its tracks.

Solidworks attempts to show you where the problems are in a sketch, but that feature is pretty ineffectual.

I draw 2D sketches that are intended for 3D very carefully these days.

Even then I sometimes have sketch problems.

One method for determining where sketch problems are is to draw a straight line across half the sketch, and trim it off.  If the problem vanishes, then it is on the side of the sketch that was trimmed off.

You can narrow down a problem area somewhat quickly using this method.

Another method to salvage a sketch is to go back and extend all the lines over each other, and then trim them all off again.

This usually clears up the problem.

A 3D program treats a sketch as a boundary, or a fence.

If there is a gap in the fence somewhere (no matter how small), or two lines where there should only be one, or one line on top of another, or a line projecting out by itself beyond the fenced boundary, then the program cannot make the calculation required to create a 3D solid.

Another way to visualize it is to think of a piece of string that has the ends fused together, so you have a continuous loop.  You can place this loop of string on a drawing board, and move it into an number of shapes (no overlapping shapes).  As long as the string is not broken, and does not overlap itself, the program will work.

A sketch must be a complete, clean, non-overlapping, continuous boundary.

.

Edit:

Another trick to diagnosing sketch problems is to temporarily cock the 2D sketch into an isometric position.

This is very helpful in exposing stray unintentional lines that are stopping the program.

I will attach a couple of examples, where I added a stray line segment up above my sketch, and another example where my vertical line extends beyond the circle.

It is much easier to see these problems with the view cocked over into isometric.

Edited By PatJ on 10/05/2022 00:54:55

Martin -

I'm afraid I'd not seen the videos but to be honest, while I am grateful that people are showing how they can draw the same parts as I'd done, they are using systems I do not know. I examined Dave's offering carefully, but was a bit lost because he refers to concepts and terms I have not met.

I have SolidEdge (CE) on my computer, but found it impenetrable.

Lee -

I don't want to get into merely slagging off programmes because I don't know how to drive them so they produce the very sophisticated work possible with them. I doubt that car enthusiast knows either, but is afraid to say so!

The TurboCAD Users' Forum Gallery is a huge collection of beautifully-rendered engineering and architectural images - including cars - showing its, and its expert users', capabilities. Far beyond what Mr A7 and I can do, but though TurboCAD has its faults and is difficult, it is he and I, not TurboCAD, at fault. Though any CAD package is hard to learn. They are designed for professional draughts-people fully trained, at great expense, to use them.

' ' '

I agree with you and Pat about boundaries around figures: it took me a long time to learn that!

' ' '

PatJ -

I have found if you are not careful, in TC at least, heavy copying, trimming and other editing without sufficient skill or care can create many line fragments and complete figures like circles, stacked below the visible ones. These can be very frustrating because TC doesn't know which one you mean. Fortunately, the pointer reveals them all, so you can weed out the dross.

' ' '

This illustrates the sheer difficulty I have using TurboCAD - NOT a judgement of the software as it was all my fault. I describe the steps I took, and the results, because clearly, I was doing things wrongly. I was not using the "wrong" programme.

I have just spent about 3 hours trying 3D again, using my engine's cylinders cut in cast-iron bar, not cast as cylinders. I need revise what I have part-made, due to problems I could not foresee.

I drew the basic block then tried to draw the covers: two discs, different diameters (compound); with a common sector cut off between the cylinders; a shallow boss on the inside face, shallow recess in the top, 6 stud-holes in each including that shared, bisected by the common cut-off. A fairly common feature, bringing the cylinders closer together.

Two overlapping sets of three concentric circles, like a Venn diagram. The cut line joins the circles' intersections. The stud holes, as circles. All still plane figures.

Trim the main outline circles to shape. Move one set a short distance away (TurboCAD makes co-ordinate and distance moves easy).

Join the arcs and cut-lines as polylines ( mind the "gaps in the fence" ) , extrude all plane shapes as required. Those generating the stud-holes project above and below, so subtracting these "dowels" leaves holes.

The recesses and bosses were fairly easy. Adjust their generating extrusions vertically from the common surface; subtract the upper ones to create the recesses.

The stud-holes cylinders were right so-and-sos though. I lost two and had to generate new ones, using temporary construction-lines to find their centres as the covers are now unsymmetrical.

Then one refused to play nicely at all; and I must admit this does hit TurboCAD quirks that are so hard to understand. I have mentioned previously that TurboCAD has at least three classes of 3D solids, each with odd characteristics. One is that if you try to alter its height, it moves up or down instead of growing or shrinking. This happened with one of the holes, making it impossible to generate it properly.

Then I "lost" one of the locating bosses - accidentally deleted. I generated a new one but chivvying it into place necessitated trial-and-error numerical moves as there were no points to which it could be snapped, and I do not know how else to have done it.

Finally I thought I would put the covers above, not on, the block - exploded diagram.

I gave up, with problems insurmountable...

First is the sheer difficulty of moving two semi-symmetrical objects in three dimensions from where I had drawn them, to other places in free space. Snap tools cannot help because those rely on defined points.

Secondly, strange events like the co-ordinates' origin no longer matching the grid axes; something I have seen occur previously. Possibly because I had switched to a facet work-plane and might not have switched it back.

Oddest was what happened to the main block.

I was trying to draw it to be made from a piece of cast-iron too narrow for plain use (giving down to 1/8 inch LP cylinder wall), so sandwiched between steel slabs which would also carry the outer cover studs and possibly the transfer passage. I had drawn and assembled the block and plates. Now, the two plates had risen vertically, like wings, to the top edge of the central block - yet I'd not touched them! Another work-plane error on my part?

.

I abandoned it, but could neither save the file first, nor did TurboCAD warn me to do so when I pressed the closing 'X'.

Well, well...

I have just tried re-opening TC. It launched straight into that drawing apparently at some auto-save point a little before I closed it. I have now saved it properly. So not lost!

And the two steel plates were back as they should, suggesting some setting had reverted to default.

' ' '

So don't let's get into name-calling that at which we may not be experts...

Those covers should be such a simple job if the first circle you draw is placed at the crossing of two axis you can then use the third axis as the centre.. Locate all other parts using that centre or simply a concentric constraint.

As for stud holes any half decent program will allow you to draw just one hole and then use a circular pattern to get six equally placed about the above mentioned ctr,

I drew the cylinder about a year ago to show how it can be done and probably the covers too back don't have time this morning to look back.

With your reluctance to watch videos or find online written manuals any software will be a slow learning process as you are blindly fumbling along rather than finding out how to make best use of what you have be it Turdbocad or any other sofware.

You could be right about TC. There are probably many who sing its praises. I am not one of them!

Out of all the "free" CAD programmes I would recommend Solid Edge to a begginer closely followed by Designspark Mechanical, then FreeCAD. Fusion 360 has too many drawbacks to make it worthwhile, and it might get worse. Are there any other free CAD packages?

What's the best freeware to draw 2D images, suitable for doing dimensioned drawings to go with MEW magazine articles?

I've no interest in graduating to 3D in the future etc. Moving off the back of a fag packet is a major step for me.

Edited By Hopper on 10/05/2022 09:25:23

It's plainly obvious that the reason for your difficulties is because TurboCAD is too difficult for you to learn. You are not getting help from other TurboCAD uses because there don't seem to be any here.

I tried TurboCAD quite some while ago and like you, found it heavy going, so I moved on. I've tried Fusion 360 as well as Solid Edge, but despite their greater capabilities in some respects I find them quite regimented in their model creation and find MoI more to my liking and for what I use it for, it is very 'fluid' in use.

You do seem to be stuck in the idea that because others can successfully use TurboCAD, then it must be a failing on your part, because you can't, but like all tools, software is there to enable to get the job done.

If a tool is blunt or broken then it should be sharpened or replaced and if a tool is poorly designed it should be exchanged for something better.

I think you are flogging a dead horse with TurboCAD and what you need to do is find some software you can work with.

Martin.

Time for some construction lines.

Draw one horizontally near the origin, so that you can see it move when you constrain it to the origin. Doing this means you know that the line is where you wanted it, not just looking like it.

Create the first circle on the origin, and the second one on the line. That enables you to add easy(and easily editable) dimensions. Do the same for one of each of the cover holes, so you can use a radial pattern once they're actual threaded holes in the solid.

Draw the outside profile of the part, dimensioning it from the origin, construction line and centre holes as necessary. DON'T use coordinates for this, for a couple of reasons: it's lots of extra work which the computer can do better, but mostly because it's what is causing your model to break when you try and alter it later. If the thing is symmetrical, you only need to draw half and mirror the other which saves time, effort and potential screwups. This is basic 2D draughting, so is well within your previous experience.

Extrude it, so you now have the solid you actually want. Work on that, creating extra planes and 2D drawings for the required features. And it should only be moved, placed, aligned or joined using the program's tools NOT moves. Because as you've found, moves are another excellent way of breaking the model in all sorts of random ways.

TurboCad is horrible to use, but all of the above applies to any of the programs.

I recommend QCAD. The free Community Edition is more than good enough for most 2D purposes, though I coughed up for the Pro version which adds various 'go faster' options such as a tool that removes line segments with one click, an operation taking 3 or 4 in Community Edition. Runs on Windows, Apple and Linux : the licence covers all of them, and multiple installations, and it's not time limited. Downloaded from here. Note the download is a 15 day trial of the Pro version, which is converted to Community by disabling the Pro features: it's the same download.

Alternatively, LibreCAD is a fork of the QCAD community edition: a little flaky when it first came out years ago, but believed OK now: I haven't used it in anger, or looked for differences.

Dave

What's the best freeware to draw 2D images, suitable for doing dimensioned drawings to go with MEW magazine articles?

With the demise of free-to-use Draftsight I moved to NanoCad, after trying QCad & a QCad derivative whose name escapes me at the moment LibreCad (thanks Dave ! ). NanoCad appeared to handle my legacy Draftsight drawings better than QCad & I could configure the interface almost identically to my Draftsight arrangement (which I configured almost identically to AutoCad LT), so there was little new learning required on my part. Where there are differences, the Help files have been adequate. The only feature I miss is NanoCad is incapable of drawing a line tangential to 2 circles.

NanoCad is a Russian product, though, which - given the current situation - may be a choice you don't wish to make.

Nigel B.

Edited By mgnbuk on 10/05/2022 11:05:06

Thanks SOD and MGN. I shall go and have a play with them.

I have just experimented with TC - SE file compatibility.

There is only one compatible of the many file-types both offer, and that is .DWG

.I opened and saved a copy as name.dwg, one of my few successful 3D name.tcw drawings - actually a slid-apart, sectioned cross-head. Then I opened that in SolidEdge. I realised it might lose details such as colour and opacity in translation. (The rendered original is in two colours.)

Though originally in 3D, only the 2D plan opened in SE. All the other views showed only a flat plane-line.

So not a good start!

Jason -

I am not "reluctant" to find tutorial material, but most of it is videos that I don't find helpful. TurboCAD came with a CD of pdf documents I can follow at my own pace.

I have two general CAD primers, but obviously these cannot describe specific makes of CAD.

CAD For Model Engineers, by DAG Brown, looks very dated by its cover photo (remember beige desktops?) and uses only 2D drawing, but does cover the basics.

The other is Neill Hughes' CAD For The Workshop - oddly using American spelling for the metre despite British author and publisher - very much up-to-date, covering both 2D and 3D to some depth. Hughes also lists the main makers of these programmes, with brief comments on them. He mentions SolidEdge but I think writing when that was still very much an industry-only system.

The problem really is not knowing what a Layer or an Extrusion is, but how to use them in the particular system you buy. They all do the same thing - geometrical plotting - but differ considerably in style and difficulty.

I copied TurboCAD's on-line 'Help' document's Contents page, and edited it by MS 'Word' and 'Excel' into a printed, proper alphabetical index written in MoD-style noun, adjective. adjective format. This greatly facilitates searching an otherwise frankly shambolic 800+ pages of the sometimes-helpful. I must admit I was very surprised I could do that with a pdf file.

Having up-rated my TC to TurboCAD 2021, I will need repeat the exercise - if it's still possible - but the document is even longer!

I have searched for other printed CAD reference-books, but found none. A dealer in second-hand technical books told me he refuses to take any IT material because it goes out of date too rapidly.

'

Martin -

I think so too! I know others who have tried TurboCAD but failed completely, making far less progress than me.

I installed Solid Edge (CE) largely after reading discussions here about it; but was deterred by the publishers' own web-site, and by it being no more intuitive than TurboCAD - less so if anything. It seemed to expect background knowledge of similar CAD systems - "synchronous" drawings? - then after a brief taste of it, leave you to it.

I would be starting from scratch. As if getting stuck machining the cylinders for my half-built engine, so starting the entire project all over again to a different design.

Also, there is the file-transference problem I described above. It would give me two incompatible CAD systems and drawing sets - and brain-fade!

.

Nicholas -

I had drawn the cylinder covers in 2D, but copied them to a new 3D drawing.

I forget if I plotted the bolt-holes by Radial Copy or construction - the latter I think, snapping copied circles to intersections; a less efficient way but same result.

I don't dimension anything by co-ordinates, but sometimes use them for working out locations. Normally I work from the (x, y) or (x, y, z) origin but place items relatively to each other by their distances, not co-ordinates.

This system also works in 3D. E.g. to put a cube on the face of another, I assemble them corner-to-corner then translate the donated one by the right distances. This is not possible if the second part is perhaps a cylinder, with no definite edge-point. Then I need to calcuIate its location because I can't grasp the proper method.

The proper TC term for translating or rotating an object is not "Move" but "Delta" or "Rot [ation]" $ n" where $ is the axis-parallel and n your typed-in value, a system with 10 possible entries in 2D, 15 in 3D; so great flexibility very easily. If I use it wrongly or needlessly is hardly TurboCAD's fault!

And two boxes called Delta D and Delta A, without axes. Not noticed those before - I don't know their purpose.

.

The one advantage I would have of moving to Solid Edge is the greater availability of help, here and in my club; but whether it is any easier to use than TurboCAD is another matter.

Another reason maybe why Nigel is having so much trouble: trying to run a marathon before learning to walk!

Nigel's wagon is a hard target for a beginner.

The wagon isn't a simple part - it's an Assembly of Parts. Not good to plunge into Assembly until reasonably up to speed creating single parts.

The wheels, axles, boiler cylinder and boxy shapes on Nigel's wagon are all Ordinary-Level objects, a good place for beginners to start.

The swept U-beam and tanks are Advanced-Level objects, not normally attempted until the basic concepts are being comfortably applied by the learner.

Assemblies introduce another level of complexity: relationships between parts: fixed, sliding, rotating, cams etc. Not a good idea to start a Black-Belt fight with an Assembly before getting a Yellow-Belt in Part building!

I'm unwilling to slag off TurboCAD or any other software without having road tested it. However, watching a couple of tutorials revealed a product with many similarities and differences to it's competitors. A few things jumped out:

• The difference between 2D and 3D operation is blurred: other software I've used clearly separates the two. I suspect the blur is due to TC's heritage, and although liable to confuse a beginner, could be useful to an expert. It would allow sketches intended to make 3D objects to be drawn with a full-throttle 2D editor, which is good provided the operator understands the limitations. I fear the feature makes it easy to draw things that look OK but can't convert to 3D. (Like Pat's lines not connecting.)
• Looks like TC displays new solids as line drawings by default. Other software makes it more obvious a new item is a solid rather than a drawing, by filling it in. (Line drawing available, but not normally used.) Again, this might be a heritage thing - older computers didn't have the grunt needed to render 3D graphics at high speed. I found it slightly confusing - is the thing on screen 2D or 3D?
• In 3D, TC allows all sorts of stuff to be done in parallel. Dimensions, colours, materials, can all be changed in the 'sketch', and several objects can created at the same time. Other software encourages one-part one sketch. My feeling is this approach improves expert productivity at the cost of confusing beginners with a million choices!
• TC seems to mixes expert and normal choices together. For example, 'Simple Extrude', can generate a solid or a surface. This is good for experts, but the beginner will almost certainly not want a surface, and if he chooses it, there will be trouble later! Likewise, the difference between a line and a polyline.

I liked what TC does, but my feeling is it would be harder to learn than the others, and they're not easy either!

On the easy to learn front, I've not had time to look at MOI yet - Blowlamp makes it look good though! Quick research suggests MoI isn't parametric like the others, which might make it more arty than engineering, but that may not matter. Dunno.

Too much to do, so little time...

Dave

Edited By SillyOldDuffer on 10/05/2022 14:24:17

Nigel,

SE will treat a DWG file as 2 diemnsional. You need to Export the model from TC. The one time I needed to export from Fusion, for opening in SE , I was asked to supply an IGES file, SE lists various file types including asm assembly documents, IGES and STEP. Hopefully, your updated TC will be able to export a suitable file type.

Gordon

Nigel, One thing that seems to have not been mentioned is that 3D design can be fun! I often design parts without having any use for them, especially flywheels with spokes. Ooo, I do love a spoked flywheel. I have even designed said flywheel, 3D printed it ( in two halves with location points so it goes back together again) and then cast it in aluminium. I didn't need the cast flywheels, so I cut them up to use on another project.