|Peter Howell 1||17/02/2021 08:27:33|
|31 forum posts|
My first foray into 3D modeling, using FreeCAD.
My question is with an assembly consisting of many parts, such as a steam loco, is it best to draw each part separately and import them into a separate assembly drawing or draw everything on the one drawing toggling the visibility of each part as it is drawn and placing it in its correct position as you go ?
|776 forum posts|
The traditional way in many places was to draw on one sheet. It was easier to handle one Elephant size sheet, later A0 size. When CAD started I continued with one sheet as we still used a large format printer. Eventually it just became easier for everybody to use a single part per drawing, historical large sheets just got cut up. Using single part allows use of smaller printer, in a lot of case a cheap laser A4 lase is good enough.
|Clive Foster||17/02/2021 09:01:21|
|2815 forum posts|
Doing it all on one drawing helps ensure that everything will fit together. If putting the nominal dimensions on a part leaves overlaps or spaces where it should touch another its easy to make corrections on the drawing.
Drawing file size may be an issue on a home computer. Big CAD drawing can make huge files. If you have both small and large parts scaling may be a problem too.
As a (still) resolutely 2D CAD guy I do individual parts on a A4 or A3 sheets and have to make corrections in metal when I've made parts that don't fit. Its harder.
One or two parts per page is much easier to handle at the machine.
My drawings generally go in transparent punched pockets to store in ring binders. I have magnetic whiteboards for notes close to my machines so the drawings can be stuck on with magnets. Still in the pockets for protection.
|Peter Howell 1||17/02/2021 09:02:37|
|31 forum posts|
Yes. In 2D draughting I've always give each part its own drawing. But now in 3D I'm wondering if it's better to have everything assembled as it goes, then separate them out later to produce a production drawing. It would mean that the total drawing, consisting of all the component part, will get very big (computer big, not physically big)
|David Jupp||17/02/2021 09:08:40|
|784 forum posts|
I can't comment specifically on FreeCAD, but generally in 3D CAD each part should be in it's own file. The file will include the material used, so mass can be derived (both for the part and later for the assembly it is used in).
Parts are combined into Assemblies. The assembly can allow movement of mechanisms etc. to be simulated.
Multiple levels of sub-assemblies can be combined for complex designs.
2D Drawings can be generated (almost automatically) from parts or from assemblies. Your drawing can be arranged however you wish - lots on one sheet, one part per sheet, ....
There are specialised exceptions to the general rule, supported in some systems.
3D CAD systems have tools to allow relationships between parts that combine together, also interference checking tools.
Edited By David Jupp on 17/02/2021 09:10:31
7473 forum posts
FreeCAD doesn't support Assembly yet. You can position a few parts manually on the same page, but it's too primitive for anything serious. FreeCAD is good at single parts (as needed for 3D printing and ordinary metalwork.)
Assembly in Fusion 360 and other CAD is far more advanced. Parts can be jointed in all the usual ways; it's easy to define a loco frame part, tell the software to feed an axle part into the holes, and then set if the axle is fixed to the frame or allowed to rotate and/or slide in the hole. Constraints and interferences are detected. Perfectly possible to assemble a multitude of parts designed by several different people into a working model that animates on screen.
Unless the model is very simple, it's better to develop parts individually and bring them together into separate assemblies later.
Sorry about FreeCAD. I'm very fond of it, but not for Assemblies.
Edited By SillyOldDuffer on 17/02/2021 09:18:19
|1882 forum posts|
Yes, methods have to adapt and change to the tool being used Peter.
With TurboCAD 2D, I used to draw everything in a single 'model' world but used many layers to do so. I'd often have a main 'GA' area and then copy parts to other areas (but on the same layer) to add smaller parts if things were getting cluttered. Views of these parts could then be made in the 'paper' world for printing PDFs etc. Of course, not being parametric - this could cause problems if I needed to modify the larger components for some reason, with much re-tracing of steps. Some of this could be mitigated by staged back-ups though.
With Solid Edge, life really is much easier in this respect. I create separate parts for each sub-assembly, then assemble them. I'm still working on my 'methodologies' in this area - by which I mean not just learning how the drawing 'tools' themselves work but the strategies (best word I can think of) to get to the desired end result easily.
Happily, SE2020 has very effective assembly methods and frankly, I'm surprised to hear that FreeCAD doesn't. The fact that SE2020 it is fully parametric also makes life simpler too.
Lot's to learn though...
21300 forum posts
When I draw up a model in CAD (Alibre) I do each individual part as a separate file and then do sub assemblies such as all the parts on the crankshaft, piston on it's rod with cross head etc and I then have a final assembly drawing of the whole engine.
I find this works out easier as if you need to go back and alter an assembly constraint there could be hundreads of them to go back through and find, it also makes the final assembly file easier and quicker to manage as file size is smaller..
|Nicholas Wheeler 1||17/02/2021 10:21:23|
|720 forum posts|
I use Fusion 360, and do the opposite; top down, where each part is modelled in place which leads to one complete thing per file
That does require careful use of components, but you should do that anyway, and I find it much easier than trying to join up lots of separate parts. You also have to consider the 10 editable parts restriction on free Fusion use.
|Phil P||17/02/2021 10:28:16|
|788 forum posts|
In Solidworks everything gets an individual identity right down to the last nuts and bolts, then these items can be brought together into assemblies and sub assemblies again each assembly has its own identity.
This is very important when you need to make design changes and record them with drawing revisions etc.
I print one drawing per part for manufacturing purposes, I only have A4 at home so that works best for me.
Here is a couple of images of my mill engine in designed Solidworks, as it currently looks.
This is a work in progress drawing of the high pressure cylinder, but this is on a much larger sheet and I need to print it at work using our plotter.
Edited By Phil P on 17/02/2021 10:33:41
|Paul Lousick||17/02/2021 11:17:59|
|1838 forum posts|
I have not used FreeCAD but have used ProEngineer and Solidworks as a professional draftsman for 20+ years. and for 99% of the time, modelled parts separately and inserted into an assembly, using constraints to fix them together, although it is possible to do it all in assembly mode.
The big advantage of making the items as separate models is that they only have to be made once and can be inserted into the assembly many times.
eg, model a wheel and if the identical wheel is used more than once, just insert it again. You don't have to draw it again as you do in 2D drawings (may take a long time to model it first but seconds to insert it into the assembly). If modelling a part in assembly mode, you can mirror it make more of the same shape in an array (a number of the same items at a common distance between them) but cannot randomly place the same part in different locations and have to model it each time.
Standard items like nuts and bolts are created once and stored in a library location and every time that it is needed, can be inserted into the assembly. No limit to the number of times it can be used and does not have to be modelled each time.
The advantage of using the same part in a number of locations is not having to model them each time used. If the part is modified, every instance of the part in the assembly is changed. If the part is used in a number of different assemblies, every assembly will be updated, saving heaps of time. This is also a disadvantage if you only want to modify the part in only 1 assembly. (in this case you replace the common part with a separate part to the others).
A big 3D model like a steam loco is best done by making sub-assemblies (of individual parts) and making a main assembly from the smaller ones. The CAD model of my steam traction engine consists 1 top level assembly and about 150 sub-assemblies, and a total of over 1000 individual parts.
2D drawings are produced from the 3D assemblies and parts, and can be in any configuration. All details on 1 sheet or spread over many. The drawings are automatically updated for every change to the models. Drawings can also be made to control the model. Change a dimension in the drawing and the models are updated (not always recommended)
Edited By Paul Lousick on 17/02/2021 11:31:07
|Peter Howell 1||17/02/2021 11:32:50|
|31 forum posts|
The latest version of FreeCAD - 0.19, (Not yet a stable release so may have bugs) has Assemblies. But even with the stable 0.18 it is easy enough to move and align parts.
I think I'll stick to separate drawings for components but import into an assembly to check for fit.
FreeCAD easily produces an orthographic (either 1st or 3rd angle) drawing on what ever paper size you want. It will also produce G-Code, though I've not tried this yet. I used to use TurboCad and Vectric Cut2D.
Thanks - It's always interesting to get others ideas. A lot of knowledgeable people out there !!
|Nigel Graham 2||17/02/2021 14:22:54|
|1666 forum posts|
A point I've often noticed missed in CAD discussions, and on TurboCAD's own forum, is that as well as a 3D fully-assembled model helping you establish clearances and accessibility, it also readily allows Exploded assembly views helping assembly, parts-listing and maintenance
Both full and exploded would work very well with the industrial practice of single drawings, paper or digital, for the entirety with separate part drawings.
This approach is necessary in the trade, using parts made by separate processes and individuals in the same factory, or scattered around contractors; and it aids commercial confidentiality.
In model engineering an Exploded view may help determine parts-lists especially for purchasing, and also time-saving by showing similar-operation components in one view. E,g. leaving turned parts for pitch-circle drilling until all such parts are ready for the second-operation sharing one machine-setting.
Phil's example above, of the orthographic drawing supplemented by a small rendering to help you visualise what you are machining, seems common trade practice too; and will be familiar to builders of the Hemingway kits.
Separate sheets have many advantages, even though they would create a formidable book of a few hundred single-page sheets for something like a miniature locomotive. On the other hand the A1 or A2 drawings usually sold for such a loco are unwieldy and some cram too much on one sheet. That was probably necessary at one time, but I ask if it has little commercial advantage with modern printing methods. (I suppose drawings could be sold on-line, but protecting their copyright might be harder.)
Many model component and sub-assembly orthographic drawings will fit A4 sheets at 1:1 or enlarged. Don't forget the Do Not Scale Drawing rubric - scaling for printing can lie irrespective of process, I think even more so with CAD and electronic printers.
(I use TurboCAD, and it doesn't offer magnifying - it might fit a 5" g. loco cylinder and its dimensions legibly at 1 : 2 on A4, but I don't think it would allow showing the drain-cocks at a readable 10 : 1 on the next sheet.)
Both Fusion and Alibre (I have tried both) intend you draw a complete 3D 'model' then it break down to the orthographic drawings necessary in the workshop. TurboCAD allows direct 2D or 3D, but I do not know if it allows extracting 2D views from the 'model'. You can though be trapped into irretrievably 'Adding' together parts that physically are made and stay separate.
Unless you are intending to publish copies you don't need all those formatted captions used on industrial drawings: just enough labels to help you make your project to your design and your facilities.
I bought an A3 printer/scanner for engineering drawings. Warning: if it's like my HP 7510, it prints A3 but its scanner is a strange <A3 size. Ink prices are a rip-off, too. That HP also takes half the evening on a noisy, bizarre self-test routine sounding as if it's about to collapse!
Do we need CAD or just want it? I suppose it depends why and how we use it, and how easily we can learn it. I bought it as a tool that could be very useful, and have found, yes, it can help you draw rapidly and efficiently what you design. Yet it can demand hundreds more hours at the computer than at the lathe, mill and bench.
It takes far more knowledge to draw and print useably by CAD, a simple engineering object; than manually, and you need much innate ability to learn CAD skill; extra to the skills of designing and making which really matter. Software publishers are not good at helping anyone learn their products. Engineering and architectural CAD is really intended for professional draughts-people taught CAD (sometimes even taught to design) in professional trade or university courses. The MEW Alibre course was exceptional in the teaching aspect; at the other end of the scale, the Solid-xxxx publisher's web-site implies being not intended for private users anyway.
I had originally taken up CAD mainly for dimensioned orthographic elevations, but hoping to create the Full and Exploded isometric views it can offer. It proved lucky that TC offers direct orthography, for I found 3D CAD far too difficult. I managed an exploded, sectional 3D picture of a simple tender hand-pump; but could have made many pumps from a fair-enough orthographical CAD drawing in the same time. Is that picture any use? As a 3D CAD exercise, perhaps. Otherwise... No.
So.... CAD has its uses in model-engineering, and I do use it thus; but I see in it a potential trap.
Creating very sophisticated 3D renderings of elaborate projects is undoubtedly a challenging intellectual exercise very rewarding to those capable of it. I accept that my CAD use is basic and inefficient, but my rather rough orthographic drawings do as intended; and I try to put the quality in the metal.
I fear though it becoming an end in itself, a massive diversion from what is just as intellectually stimulating but arguably more important: actually designing and making the physical models. My workshop session today will be finishing a chuck-adaptor needing only a few measurements. No CAD at all.
|Peter Howell 1||17/02/2021 15:50:36|
|31 forum posts|
The discussion my query provoked has be most interesting.
Personally I get a great deal of satisfaction from producing a good drawing, and you can do it sitting down in the warm !
I have enjoyed Technical Drawing (as it was called) at secondary school. I still have a book given to me as a school prize for that subject. Then in the early 1980's I introduced a very early CAD system into the small engineering company I was working for. A program called RoboCAD running on an early IBM PC. I was still involved in producing drawings for them up until I retired in 2000. But only in 2D. After that I bought my own copy of TurboCAD and continued producing drawings for my own use - but to a reasonable standard.
Now I thought it about time to stretch the grey matter and try to get to grips with 3D. FreeCAD is free so nothing to loose if I give up. I have been told I should have signed up as a hobbyist for Fusion360. But I'd already started producing some stuff with FreeCAD.
|Nicholas Wheeler 1||17/02/2021 17:27:28|
|720 forum posts|
You have that completely back to front: just explaining the conventions for representing 3D objects on a flat piece of paper takes far more explanation than being able to orbit around a '3D' object on a screen. Fusion even names each of the six faces Front/Back, Left/Right, Top/Bottom which requires no explanation, and clicking on those rotates the object so you're looking directly at it. One simple sketch can provide all the information to produce a 3D part like a single cylinder crankcase. A quick outline, constrain the geometry, add dimensions and extrude - the same work as drawing just one face. You add features like holes, slots, bosses directly to the face they sit on - what could be easier? And that's before you start on more complex operations like lofting, sweeps, sections, surfaces or moving parts that are very difficult to do on paper.
This all dramatically reduces the skills that a designer needs to create complex and/or multi-part objects from scratch. Creating a 2D drawing is then a simple operation if it's even needed at all; many parts can be made on manual machines from the information directly available from the 3D model.
I had an hour a week of Technical Drawing when I was 13, 37 years ago. That leaves me able to read a drawing, but designing parts in 2D would take me months of instruction, practice and frustration before I ended up with something usable. This model is completely dimensioned, animated with all the clearances worked out over a couple of evenings:
It means that the flat parts can be laser cut from the model, thus saving even more time.
Edited By Nicholas Wheeler 1 on 17/02/2021 17:32:46
|Peter Howell 1||18/02/2021 09:06:43|
|31 forum posts|
Surely in TurboCAD when you insert a view into your 'Paper' Space you can change the scale. So all you need do is create a separate view of the detail, insert it into Paper than increase its scale as much as you need.
I've just checked this. I am running an old 2016 version Turbo that I've never transferred to my new Laptop so I had to fire up the old computer and checked last night.
7473 forum posts
I use both! Though fluent in Windows, I prefer Linux, which Fusion 360 doesn't run on. Apart from that, I find FreeCAD "better" for single parts, though that may be because I learned FreeCAD first and am used to it.
Although Fusion is powerful it has negative features. (All tools have negative features!)
FreeCAD's negatives are being relatively primitive with a future depending on dedicated maintainers rather than a well-funded commercial operation, but it is genuinely free, and runs locally - no cloud!
Not sure if it's a plus or minus for FreeCAD, but whereas Fusion focuses sharply on mechanical engineering, FreeCAD has Architectural, Ship Design and a bunch of other CAD 'Workbenches'. So many choices confuse the beginner and I'd selfishly prefer the developers to concentrate on improving the tools I use!
Thanks for news of FreeCAD v0.19pre and Assemblies, especially as it turned out I was running v0.17 when FreeCAD's latest stable release is v0.18.4 Done an upgrade, and will keep an eye on 0.19!
|1882 forum posts|
You may have already set sail in this area Peter - but I started to move from TurboCAD 2D last year and discovered Solid Edge 2020 - which is free to download (with a lifetime license) and is not cloud based.
The only thing I'm aware of that Fusion offers (that SE2020 does not) is a CAM facility. This is not an issue for me currently (no CNC, only 3D Print) and I am really delighted with Solid Edge. If you eventually find FreeCAD is not for you - I would very much recommend trying Solid Edge 2020 next.
Edited By IanT on 18/02/2021 12:44:30
|Phil P||18/02/2021 14:23:18|
|788 forum posts|
Edited By Phil P on 18/02/2021 14:23:34
|71 forum posts|
For what its worth I use Onshape - its a cloud based CAD package from the original developers of Solidworks. I create parts from sketchs - how many parts I create in on sketch tab depends on my mood. These are then combined into an assembly with various constraints applied. Drawings can then be produced from individual parts, sub-assemblies or assemblies.
There is no limit to the size or number of models you can have other than a 'free' user's models are available to any other user to copy. Unless you wish to retain some IP in your drawings that isn't a problem.
I think its a brilliant piece of software.
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