3D cad design sequence

[GreenTwin]

I still am confused on how to actually start a new design. I can see creating individual parts but without an overall assembly I have no idea what those parts are going to fit.

You create one part file for each part, and when you get all the parts done, or even before you finish all of your parts, you can create a separate "Assembly" file.
In the assembly file you can drag and drop one of your parts at a time.
Generally you want to "fix" the first part you drop into the assembly space, so that it does not shift around as you are mating other parts.

Lets say you insert the engine frame first, fix it so it cannot move, then insert the crankshaft.
The crankshaft will come in at some random angle and position, and you can drag and rotate it around so it roughly aligns with the bearings in the frame.
Then use the "mate" functions to make the crankshaft concentric with the inside of the bearings.
You pick the mate, concentric, pick the crankshaft, pick the inside of the bearing.
The crankshaft will move so that it aligns with the inside of the bearing.

Then use one more mate function to mate one of the surfaces on the crank web with the inside of the bearing shell.
The crankshaft will slide over and should be in the correct position.

Then you should be able to use the mouse to rotate the crankshaft in the bearings, and you can check to see if the webs clear the frame as the crankshaft rotates.

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[GreenTwin]

In this example, I inserted the frame part into the Assembly file first, and fixed its position.

Then I inserted the crank next and mated it to the bearings, then mated the flywheels to the crankshaft, added the water hopper, muffler, gears, rod, piston, etc, ading one part at a time, and mating each part into the correct position.

Once all the pieces have been inserted and mated, you can explode the assembly, to look like the image below.

If you make the cylinder inner and outer surfaces translucent, then when you rotate the crankshaft, you can see the piston move back and forth, and you can verify the piston has the right travel and does not strike the head.

Here is an example of a translucent crankcase.
I can rotate this crankshaft and watch the pistons move.

 

[Jasonb]

To some extent is does depend on what you are designing, the approach for replicating something from old photos will be different to that for a new design of barstock engine. I've already outlined the former

If I'm designing from scratch or heavily modifying something I have a good idea of what I want in my head before I even turn on the computer as it's the user that needs to come up with the design, the CAD is just a way of detailing it and checking it works before cutting metal.

I may again have a doodle on a scrap of paper or as Chuck says lay out some basic positions with Alibre in the form of a 2D sketch. About midway along the Alibre tool bar when in sketching mode there is a green dashed line with more options in the drop down, they are good layout lines for things like engine ctr line, base height, etc and you can ad points and axis and then even build up a crankshaft and conrod as little more than lines and then try out the geometry at an early stage. You could also do a guide circle if you are fixed tt using a set size flywheel and then proporting the rest around that.

Moving on from that I produce simplistic parts and then flesh them out as the design progresses as it's easier to alter a part that has just a few sketches to make it up than loads of detail. So say for a con rod I may simply sketch a rectangle with a hole at each end and then extrude that to give it a bit of thickness. This can then go into my assembly to check for movements and fits and once happy I'll use the hole positions and detail the proper conrod around them

 

[Zdenek Hadrbolec]

How do folks design something in 3D? I am thinking something like a single cylinder engine. I am envisioning a sequence like perhaps drawing a piston, a crankshaft and a connecting rod kind of out in space and adding things like a cylinder and frame for mounting the crankshaft etc. all rather crude and without detail. Then once you have the major components in position you would make detailed refined drawings of each piece and insert the refined piece back into the original assembly. I am used to designing in 2D where I would start with an a crude assembly drawing with probably front, top and end view and then making a detail drawing of each individual piece and modifying the original assembly drawing to add the details. I am not sure of how to make a similar assembly drawing in 3D and then refining the individual pieces and replacing them in the original. I guess I am asking a chicken and egg question. This 3D stuff is new to me and I am kind of old to learn new tricks. I started with pencils and triangles etc. back in 1962 and gradually progressed to cad but sold my business and retired (several times) in early 2000's.

Your idea is unnecessarily complicated. It's much easier. Personally, I proceed by first determining how big a propeller I want to use on the model. The diameter of the propeller defines for me the approximate power of the engine, these values have been known for a long time. The corresponding performance is also related to the stroke volume. This is the product of the piston diameter and the stroke. Most fast motors are undersquare, I choose a slightly oversquare ratio in my designs. Well, when the stroke of the crankshaft and the diameter of the piston are known, I start modeling. First I will create the piston in all the details. Below it, for now without defining the mutual distance with the piston, I will create a connecting rod, or rather its crank part. I define the size of the connecting rod and its distance from the center. I model with the pin position at the top. Then I copy the crankshaft model and rotate it 180° with the pin down. I switch between the views of both variants as needed. I will pull the piston to this model with the pin down and position it so that there is as little gap as possible between the flywheel and the piston. This gives me the axial distance of the connecting rod and piston pin, this dimension defines the actual size of the connecting rod. I will model the connecting rod right where it belongs. If some models (piston, crank) get in the way, I will temporarily hide them. When the connecting rod is done, I visualize the crankshaft with the pin on top, make a copy of the piston and connecting rod, and move both to the correct distance. That way I have the top position of the piston defined and I can create the cylinder liner and the cylinder itself. Then I create a sketch of the engine head in section, determine the size of the combustion space according to the type of engine (diesel, petrol) (calculation according to the relevant literature) and when it is finished, I create a model of the head by rotating the sketch along the vertical axis. The rest of the engine is then routines such as bearings, covers and so on. Simple. (I model a nine-cylinder radial engine with a built-in starter for about 12 hours, a small simple five-cylinder engine for about three hours)

 

[kvom]

When making an assembly, the initial part selected is fixed. Any motion in the assembly is relative to the initial part. However, when making assemblies from other assemblies, the included assembly needs to be marked flexible so that the base part can move relative to the other assemblies. If this isn't done it may be impossible to make the model move.

Petertha's remarks on mates is on the mark. It's perfectly possible to design parts that can't be assembled in real life. Even when the software determines that there are no interferences, assembly order needs to be thought through.

 

[Richard Hed]

In this example, I inserted the frame part into the Assembly file first, and fixed its position.

Then I inserted the crank next and mated it to the bearings, then mated the flywheels to the crankshaft, added the water hopper, muffler, gears, rod, piston, etc, ading one part at a time, and mating each part into the correct position.


View attachment 141449



Once all the pieces have been inserted and mated, you can explode the assembly, to look like the image below.


View attachment 141450


If you make the cylinder inner and outer surfaces translucent, then when you rotate the crankshaft, you can see the piston move back and forth, and you can verify the piston has the right travel and does not strike the head.

Here is an example of a translucent crankcase.
I can rotate this crankshaft and watch the pistons move.

View attachment 141451

What program are U using for this?

You guys need to tell which program you are using when speaking of what you are doing. I find that each program I use works differently. In one program, what you might be saying, makes sense, but in another, that would not be how it works. I mostly use Alibre and AutoCAD Architectural 3D 2004i.

I thimpfk that A-CAD has some very powerful stuff in it, but I have moved over to Alibre because, altho' less powerful, is MUCH easier to use, and FAR easier to create a 2D.

 

[Gordon]

I am starting to figure out how to produce the individual parts. I think that my past experience in 2D is actually a big part of my problem. I expect Alibre to be able to do things the same way Visual Cadd could do it. I think that making a rough assembly/section view with Visual Cadd to get the overall profile fixed and then making the individual components in Alibre is actually the way to go. As was suggested, making something like a crankshaft can be nothing but a rectangle in the initial 2D concept is acceptable. The fine details can be added as the design progresses. Things like bearing housing and cylinder liner etc. are not required to check concept. The idea of starting with individual parts and then adding them to an assembly seems backwards. I have to know if I am designing the parts for a tank or a lawn mower and it is still true that two pieces cannot be at the same place at the same time.

 

[Richard Hed]

I am starting to figure out how to produce the individual parts. I think that my past experience in 2D is actually a big part of my problem. I expect Alibre to be able to do things the same way Visual Cadd could do it. I think that making a rough assembly/section view with Visual Cadd to get the overall profile fixed and then making the individual components in Alibre is actually the way to go. As was suggested, making something like a crankshaft can be nothing but a rectangle in the initial 2D concept is acceptable. The fine details can be added as the design progresses. Things like bearing housing and cylinder liner etc. are not required to check concept. The idea of starting with individual parts and then adding them to an assembly seems backwards. I have to know if I am designing the parts for a tank or a lawn mower and it is still true that two pieces cannot be at the same place at the same time.

I thimpfks that eventually, you will find that your 2D experience is actually "in the way" of you learning Alibre. What you say may be true for "concept" but I find that in Alibre, you can build your "concept" right off. If it isn't right, you can adjust it or simply start over very easily. Once in a while when I have something very complicated, I have to delete some feature and start that feature again.

But, I'll tell you what, some things the guys here have been saying are news to me and I am finding Alibre to be even more powerful than I thot.

 

[Oldiron]

I too have lost access to Auto CAD and am trying to learn Alibre but the work flow is Greek to me. A simple thing I"m trying to draw is a 4" pipe with 1/4" studs sticking out at right angles, like a pissed of porcupine, to hold tool holders. Are you saying I should draw the pipe and extrude it in one drawing and then make the studs in a separate drawing and then combine them in a third assembly drawing? Draw bearings to rotate the whole thing, add them to the assembly, rinse and repeat for each additional part. Something complicated like a V-8 engine might have a hundred part drawings and one assembly drawing? Bob

 

[Jasonb]

I would draw a circle centered on two axis as my first sketch and extrude that to form a solid cylinder.
Then another sketch on one of the planes passing through the ctr of the cylinder of your stud and then extrude that stud to a length so it sticks out beyond the cylinder.
Then use linear and radial patterns to add multiples of the same stud
Finally draw a circle the diameter of the bore on one end of the cylinder and cut extrude that to now make it a tube.

 

[Jasonb]

Here you go. It's all treated as one 3D part but made up of sketches not drawings ( drawings are the 2D workshop drawings at the end

Basically what I said above but I extruded equally about the mid point and added a mirror before the linear pattern. There are a couple of other ways to do it such as sketch two concentric circles first and extrude to form the tube. Then add a plane some distance from the side of the tube, draw your stud or studs on that and extrude to the edge of the tube but the way I show is simpler to start with. You could also use the pattern feature to sketch a row of circles and then extrude the lot in one go.

You may want to use pause or select slow motion to take it all in.



That's the way I would do it for my own use but you have actually got 11 parts there so you could draw the tube and then instead of extruding the stud as a solid use cut extrude to put a series of holes in the tube.

You would then create a separate part for the stud

You can then bring these together as an assembly

Finally you would produce a working drawing of the tube dimensioning hole size and position. Another drawing (or put two parts on the same sheet) for the stud and call out 10No required. Finally an assembly drawing with all the studs in place dimensioning how far they stick out of the hole and maybe calling for a welded joint.

 

[Bentwings]

I agree. When the lace I worked at went paperless there were very few drawings in the shop the few manual parts being made were almost custom parts . In the model file we just used the drawing formate as a not page where special considerations were noted Maybe a welding note or something like that the cnc program kicked out orders for tools not in the tool changers as engineering we didn’t event have to worry about ordering special tools the cnc shop knew what they needed so they took care of all that on rare occasion they would call and say “ mr. “ engineer is it ok if we use a tool that gives a better finish or can we use a different material . But that was very rare the machines were so precision that tolerance was not an issue . You built it in to the parts if you wanted more clearance. There were very few precision ground parts . Something like that might be sent out but that was very rare. We might source special materials but that was noted on the bill of materials page . That was auto generated too there were some standards but thankfully that old book got tossed out. The biggest problem was that most new engineers had no experience in the shop so they might model something not possible to make Putting openings and holes in inaccessible positions was common for them. Our progress meeting usually solved issues quickly . Initially the company had basic construction standard and rules a really big book all from the old days
Don't confuse drawings with sketches.

A "sketch" is the base shape that you create (like the PlayDoo die), and you use that shape to either extrude or cut into a 3 dimensional object.

A "drawing" is something you create using your 3D program, by dragging and dropping a 3D model onto a titleblock or border, or dragging an entire assembly onto a border.

Once you start using 3D modeling, you no longer create any drawings; the 3D program does that for you when you drag and drop models into a border.

If you want to change the drawings, you change the 3D model only, and those changes are automatically reflected in your drawings that you created in the 3D program, in every view (and thus the parametric or linked approach for 3D modeling).

The power of the parametrics of 3D modeling cannot be understated.
Parametrics is like the invention of the wheel, or the striking match; or the airplane; it changes the design process dramatically and forever, for the better.

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[GreenTwin]

This is an example of using some mock-up parts to verify run of an engine, in simulation in Solidworks.

This is a really powerful feature, and fun to see a run preview on the screen too before the engine is even built.

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[GreenTwin]

Here is a single part that is rather involved.
I am still working on this one (Soule Speedy Twin twin steam engine frame).

I started with the cylinders, and just kept working outwards, sketching and extruding.


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[GreenTwin]

3D print.

This engine will be cast one day hopefully.
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[johnmcc69]

Great post Gordon! This (3D CAD) is all like trying to eat an elephant...

As you mentioned (& others) you might be better off designing all the individual parts & then later creating an assembly file with all the parts in it. I wouldn't worry too much about using the simulation & collision detections if you're just trying to learn the software, get the basic workflow down first. I'm a Pro-E/Creo user & when I was learning to use the software (at work, designing tooling...) I bought a couple books (SDC publications, many years ago, I'm not sure if these are available for Alibre, but I'm still "old school) & would rather have a book in front of me rather trying to pick out all the commands in a YouTube video. I also started drawing up "proven designs" (Very simple ones), mostly Elmers engines or simple oscillators just to figure out how to use the software, one part at a time. I then figured out how to do the simulations, ETC. Because a model with lots of parts gets very ugly if you screw up the "assembly connections" & will make you want to give up (but don't). After doing some simple models, you will see what is required to set up BOM's & create some good working drawings.

After you've gotten to this stage, you'll probably have built some engines (I know you're a good designer).

&, after you've reached this point you'll start pushing the software a little more.

I "Think" Alibre (& other softwares) have this function, but you can create a new part within the context of an assembly to use existing geometry as references. The reference was made earlier in this post about if you change the "size of a crankshaft journal" you would have to remember to accordingly change its diameter. Well, If I create the bearing in the assembly context (This becomes it's own stand-alone part) of the assembly, & use the crankshaft diameter as a reference, I use that diameter & offset it by say .001" off that dia. for the bearing, that bearing will update accordingly & ALWAYS give a clearance of .001". If I change that dia. (Crankshaft) by 100" or .003" (extreme example, but it works), it will always maintain a .001" clearance.

Constraints are REQUIRED. In my last example, if you did not use them, you would find a lot of problems, especially "downstream". Parts MUST be FIXED, with the exception of "mechanism" parts. This technique also works for bolt patterns in assemblies. A couple of examples, if I assemble a crosshead part to my cylinder (That already has the bolt pattern, & orient it correctly, I can (in the assy. mode), "activate" my cylinder & use the bolt pattern to create the tapped holes in the cylinder (using the axes of the crosshead). If done correctly in the crosshead & the holes were created using a "pattern", I only need to create ONE hole in the cylinder & then use "Ref. pattern" to copy the holes EXACTLY to the crosshead. This doesn't matter if it's 6 holes or 60, it will ALWAYS follow the "Pattern" of the crosshead & I don't need to do the math. 'cept maybe the tapped hole size...

Importing ACAD 2D sketches into 3D has always been a bugger for me, lack of "good" geometry (open ends, non constrained. polylines...). I've given up doing that & just re-create it in my 3D sketcher.

Another note about creating the 2D sketches to create 3D geometry... don't over complicate sketches. If I create a piston, I "Revolve" my piston dia. & that's it...I create the ring grooves as another revolve feature (this all goes back to constraint's & dependincies. For instance, if I want to modify the ring grooves from the piston, I just need to edit that particular feature without touching the piston sketch.

Phewww...

Don't be overwhelmed Gordon, but start with the easy stuff.

Plenty of well qualified help here to help you on your journey...

JoHn

 

[GreenTwin]

I think John is saying this in his post above, but he brings up a good point that I had forgotten.

The question was asked "How do I design the engine so that all the parts will fit?".

I sketch the first part, and then I can copy that sketch, and start a second sketch and part, and like John said I can use the same hole pattern or shaft size and sketch to begin a new part, and so I know the parts will fit because they originate from the same sketch.

Another trick I have discovered is if two parts are very similar, then save Part 1 and Part 2, and then suppress some pieces of Part 1 to create Part 2.
No need to actually create Part 2, just supress a few things and leave it like that.

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[Gordon]

I am sure that my biggest problem is that I am used to 2D and I am having a problem trying to adapt to a different way of doing things. Even the mouse buttons do not work the way I am used to.

I am trying to work on a V twin which I obtained PDF drawings for from another forum. I drew them in my 2D cad because that gives me a better understanding of function and fit etc so I know what I am aiming for. I am having a problem with having my sketch fully defined and that means that I cannot go to the model to extrude , copy etc. I do some operation and the next time it does not work. I have watched some YouTube videos but it is hard to follow them because something happens and I am left wondering how did that happen?

 

[johnmcc69]

Gordon, like I mentioned, your sketch may be too complicated. Start with a simple cylinder & add fin's, fillets, dtails later. You can go back to those at any time & add features.

john

 

[GreenTwin]

I distinctly recall when learning 3D modeling that I would continuously get "stuck" when trying to do something.
I would make great progress, and then hit this insurmoutable barrier.

Sometimes it would take days or even weeks to figure out what was stopping me.

Or my model would be going well, and then it would suddenly blow up.
In the beginning, I would save a different version of each part every hour or so, in case things blew up, I could open one of the earlier attempts.

The beginning of learning 3D modeling is like learning to ice skate (for me).
In the beginning, you keep falling on your face, and begin wondering why ice is so good.

I can say that learning 3D is well worth the struggle, but it is a mind-bending struggle (or was for me).

It is really unreal the things you can design with 3D once you get a feel for it.

I do recall asking questions on forums about getting stuck in 3D, and getting answers, and I still do this to this day.

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