Multiple coincident constraints overlapping one another?
"I have never developed a full, solid understanding of how Fusion decides whether a constraint is a diameter constraint or a radius constraint, so I just work with whichever it gives me. (The best rubric I've ascertained is that a "whole" circle gets a diameter and a "partial" circle gets a radius, and then, once written, it stays as either diameter or radius"
That is the rule for the default for diameter vs radius. However, you can always change it after the fact, by right clicking:
"I'm struggling to see what I lose doing it this way. OK, my sketches are a little more crowded with the additional constraints. But even so, with the function/value references, I can still change the diameter of all holes by simply changing one of them."
"To me, it seems like a question of, "Do you want everything in one box (i.e. the sketch)?" or "Do you want spread the complexity over multiple boxes, but have every box contain as little as possible (i.e. minimalist sketches, accompanied by a bunch of patterning features)?" Am I missing something? This feels like a to-may-toh/to-mah-to thing to me."
To some extent, yes, it is your choice. You can have very complex sketches, including patterns and symmetry, but what @TheCADWhisperer and others are trying to say is that you might have a better experience using more, smaller sketches. The larger a sketch gets, the slower it gets (the solver has to solve all those constraints and dimensions), and to some extent, the more unstable it gets. But, yes, in the end it is certainly your choice which way to go.
"FWIW, I have found that Fusion is a lot easier to work with when you know exactly what you intended from the get-go, and that the times when I've 'figured it out as I go' usually end up in a from-the-ground-up redesign once I figure out what I wanted"
Yes. This is not limited to Fusion, but is true for any CAD system. You will always end up with a better design (and it will take half as long) if you do it twice. Even experienced users find this to be true. Over time, you will gain some insight, based on past insights, and find that you need to start over less and less. Many CAD instructors teach that you should ALWAYS plan to do any non-trivial design more than once. I'm no CAD expert, but I have spent a lot of time designing and modeling stuff in Fusion and Inventor, and I often find that I need to start a part or entire design over once I realize what parameters I want to change, and even what set of features I want to use to model it.
Jeff Strater
Engineering Director
@ipmcc wrote:Yeah, let's do this thing!
This is a simple design - but I think it can be used to illustrate where you can change techniques that will significantly benefit more complex designs.
I am going to go through this slightly differently than how I would actually do the design for the purposes of illustrating the logic.
I will explain some logic as I go and leave other explanations of logic until the end after it is all completed.
Step 1.
Sketch a circle at the Origin and dimension (either as Diameter or right click as Radius as shown by @jeff_strater).
Now sketch a 2-Point Rectangle selecting approximate Points 1 and 2 on the Circle.
Add a Coincident Constraint at Point 3 between the Rectangle corner and the Circle.
The Rectangle is now centered.
Now add the two dimensions to the Rectangle as shown.
The second dimension will prompt you that it isn't really needed and will create a (reference) dimension in parenthesis.
I worked for 8 years out on the shop floor making actual parts from 2-D drawings.
I would go to the stock rack and pick the round stock.
To cut the flats it would be all but impossible to measure the 175mm dimension that was in your original sketch, but trivially easy to measure the 65mm dimension.
Delete the 175 dimension - it doesn't make logical sense.
Right click on the 60 dimension and select Driving.
So now the 60 controls the Rectangle and is easy to measure and manufacture on the shop floor.
Select the two vertical lines of the Rectangle and hit x on the keyboard (or right click - right click everything) to toggle to Construction (dashed linetype).
Now, DON'T trim the circle. Remember the formula for a circle from HS math class? The circle is defined. If you trim it, the geometry would be more complex 2 arcs with 4 endpoints.
Extrude the profile midplane just as you did before.
As we go through this, we are going to create one and only one sketch - just as you did before.
Next, we will look at the Sketch Slot command...
There is much much more to investigate in this so stick with me, but my wife wants to go to the beach (I am retired in Hawaii, just do this for entertainment) so I will have to stop here for a while... ...check back.
We will take a look at Fusion AI too.
Next, let's discuss these 6 dimensions (the geometry requires 6 arcs, 6 centerpoint coincident constraints for the arcs and 12 endpoint coincident constraints).
Ever taken a programming course? I'm not programmer - but I have taken a couple of beginner classes back in the last century. It would be a nightmare just to write a program to error check all of these parameters). One circle with one centerpoint will suffice as far as the program logic is concerned. Might help the human to visualize but doesn't help the computer to have all that extra geometry.
We could argue that this would be better done with the Hole command, but we will follow the original and Extrude a circle.
But before we continue - this geometry does not look aesthetically pleasing to me (customers like aesthetically pleasing sometimes more than function).
It would also be more expensive to manufacture as originally designed (unless all you ever do is 3D Printing).
Do you have to have the dimensions as specified in the original design,
or can we alter the design to make this larger circle Tangent to the smaller circle?
The difference amounts to about the thickness of a sheet of paper for the larger circle to be a bit bigger (Tangent) but reduces the cost and improves aesthetics.
We will do whatever you answer.
I just realized that another option would be to leave the circle at your specified size, rather than change to my suggested Tangent size, but not trim and would have these divots.
"I see no reason to prematurely optimize my sketch to make things easier/quicker for the Fusion solver, unless/until it becomes too slow for me to tolerate at my 'speed of mind'"
this is a good plan. However... Once you get to that point in a Fusion sketch, it can become MUCH hard to optimize later. If you have a single large sketch that eventually gets to the point of interfering with interactive usage, breaking it into multiple sketches will then break any references to geometry in that sketch. So, as long as you get to that point of intolerance before you consume it, you will probably be OK with that plan. But, once you consume a sketch with features, deleting any consumed geometry will cause many worse headaches than a slow sketch will. This is where your analogy to optimizing software breaks down. You can easily split a 1000 line function into 10 100 line functions, and, as long as you do that carefully, nothing bad will happen. The closest analogy I can layer on top of yours is: If you used gotos in your code, where the goto target was a specific line in the text file, then, when you refactor, all of those gotos will have to be edited to jump to the correct place in the newly refactored code. Of course, that example is nonsensical (no one uses gotos, much less to a line number), but hopefully you get the idea.
That is all we are trying to tell you here. Yes, I understand that changing the way you work because of the tool is not ideal. It would be great if Fusion could support many widely different working styles, all of them without losing efficiency. But, that is not the world we live in. All tools work better if you use them as intended. I have used a visegrip to pound in a nail, because I was too lazy to go get a hammer, but, really, a hammer would have worked better.
Jeff Strater
Engineering Director
Are you familiar with Grace Hopper's work.
My interest is who/how is the AI going to be trained?
Most users here don't have the slightest interest in learning how to do things "right" and will accept work that is not only not aesthetically pleasing but is also not functionally ideal and certainly not computationally efficient.
Edit: I forgot to mention that editing a sketch pattern does not update to the features. Another powerful reason to Pattern Components, Bodies, Features, Faces rather than sketch elements. As in many things, there is a good, better and best way of doing things. And then there is also rubbish... ... you never addressed the quality questions in your design.
