Fusion
Howdy Gurus,
Suppose you have the following geometry:
And you want to create a fillet between two lines to the point where it is coincident to the circle. How do you do that?
Thanks
John
The key word here as @TheCADWhisperer has already mentioned is tangency,or the tangency constrained.
Another thing you might want to consider is that it might well be easier to design your 3D object with harp edges and then apply fillet features to the edges. Not only is that often faster to design, It keeps the sketch simpler and more stable and also has performance advantages.
Well I thought so too, and that's what I tried at first. But when I tried applying the tangency constraint, the drawing got all weirded out-- but that was on my more complicated drawing, perhaps there was something else wrong...
I just tried it on my simplified drawing and it sort-of seems like it *oughta* work, but in reality it doesn't. Here is a screenshot. I tried it twice with two slightly different setups. The first attempt (not shown) I did not set a formal radius on the center circle. When I applied the tangency constraints it sort-of worked, but only because it yanked the radius of the circle-- made it larger, and several of the lines were extended beyond the frame of the rectangle, similar to the way they are in the screenshot below.
For my second attempt, which the screenshot depicts, I reverted to the same original setup, fully-constrained the circle with a formal dimension and then added the fillets and constraints. With the circle now unable to adjust to the fillet, the operation failed, though the fillets were formed and extended the boundary of the rectangle again as in the first attempt. If the operation had worked, I could live with the extended lines and simply ignore or trim them off. But as you can see, the tangency constraint did not actually work. (Also ignore the section that is a construction line-- I didn't notice it until afterwards and it makes no difference to the end result.)
ALSO AS A FOLLOW-ON QUESTION -- Is there a way to create the fillet without losing the original lines the fillet is made from? In my drawings I have had to redraw the lines over and over for each new fillet.
REGARDING FILLETS TO 3D OBJECT -- Normally that's exactly what I would do, however in this case there are so many to apply that I thought I would just take care of it in the sketch. Without intending to sound offensive, my naive question back would be how can Fusion 360 claim to be fully parametric if this cannot be dealt with effectively (ie. "stably") from the original sketch? What am I missing?
Thanks for your assistance and guidance. It is much appreciated!!
John
If you want to see my full drawing, here it is, although I don't think that it shows anything different from my simple illustration. They both seem to react similarly to the fillet / various constraints when applied. And I did try to use the tangent constraint at first-- and when I was doing it, it sorta seemed like it should work, but in the end, it made the lines wonky and I ended-up not doing it that way. I just put in fixed-radius numbers for the fillet. But that means if the center circle changes diameter, all of the fillets have to be recalculated.
John
Can you export your design and attach it as a .f3d ?
Also, can you highlight those areas in the sketch that you want to create 3D geometry from ?
This is exactly one of those sketch problems that can be very timely to solve the sketch environment.
People have the tendency to create sketches that precisely reflect the outline of the geometry that they wan to create.
That applies to new users as well as to many experienced veterans and for the latter it might well have to do with how CAD software has been developing thought eh decades.
However, he problem with that approach is that when filleting, breaking and trimming sketch geometry often existing constraints are broken and other's have to be re-created. Debugging such a sketch can be very time consuming and occasionally you also might encounter a bug.
Here's the same component with a lot less sketch work and a little more in solid features.
The holes I farmed out into a couple other sketches.
See the second component in the attached file.
Here's another idea just in case you need to specify the wall sections and don't care about the actual radius in the corners. Note the 2 construction circles and the tangent constraints. When you add the dimension between the circles, start the dimension command then right click and select Pick Circle\Arc Tangent.
File's attached. I only drew a quarter then used 2 mirrors, I haven't finished adding the fillets etc.
Mark
Mark Hughes
Owner, Hughes Tooling
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I understand what you're saying, and that is a nice version of my drawing-- and it works as long as it's symmetrical-- which in this case it happens to be-- so you can use the mirror tool to save yourself some work. What I don't see / understand is how you are able to control for this bit (highlighted in red in the screenshot), which should have a nominal and specified minimum thickness?? When you do it in the sketch it should be able to be specified / guaranteed via a constraint to conform to / and hopefully be controlled tangentially through the diameter of the circle. But when you do it in the 3D mode, how is the thickness guaranteed?
I've examined your drawing several times and I don't really understand how it's appreciably different from the things I've already tried? There is no substantial difference between a "real" circle and a "construction" circle is there? Apart from one being included in the final result and the other simply used for hints...??
I've tried a number of times today, since my last post this morning, to recreate my drawing from the sketch mode and I keep running into various issues such as legs being constrained (when creating fillets) which interfere with the ability to apply the tangent constraint and so forth.
The mode of drawing that has gotten me the closest to success, where I've created stub line segments to use as starters for each of the fillet operations. I've tried completing it a number of times and always end up with issues of over-constraint and the like and cannot get it completed. The one that you see here will not be constrained using the tangent constraint. If I remove the dimensions from the lines, the tangent constraint will work, but then the lines refuse to be constrained by the dimension tool. So I'm screwed either way I go.
First only draw a quarter of the design, your sketch with the whole design was unworkable because of too much geometry.
I'm not really sure what you want but you can't add tangent constraints if you have the fillet radius defined. You have the 3 sides constrained 1mm from fixed lines and the fillet radius is defined so there's no way you can add the tangent. If you delete the radius dimensions you can add the tangent you need to decide which one you want to define. The construction circles I added where just to allow you to specify a minimum wall section and then make selection of profiles easier for the extrusion.
Mark Hughes
Owner, Hughes Tooling
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@Anonymous wrote:
I understand what you're saying, and that is a nice version of my drawing-- and it works as long as it's symmetrical-- which in this case it happens to be-- so you can use the mirror tool to save yourself some work.
If you have a part without symmetry and a lot of pockets like this then use more than one sketch. A couple of reasons why, one the sketch engine will not slow down and two with a sketch like this in not easy to figure out what's going on.
Mark Hughes
Owner, Hughes Tooling
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Here's a screencast showing how I'd draw the pockets. Don't know if you've figured out the line tool draws arcs if you click and drag. I haven't drawn the construction circles this time as I don't know what wall sections you need but this should give you an idea.
Mark
Mark Hughes
Owner, Hughes Tooling
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The purpose of my post was not to perfectly recreate the design intent in your model.
The "busy" sketch in your model also makes that more difficult to read.
The purpose of my post was to clearly demonstrate that with a little re-organization your model it lends itself perfectly to use more solid modeling features and thus substantially reduces the time it takes to create the sketch, regardless whether it it symmetric or not.
It also substantially increases the stability of the model. This might not be apparent is a single component, but if you are working on a more complex assembly this will make a substantial difference in the behavior of parametric models.
As such picking up the right habits when starting with a new discipline - parametric modeling in this case - will go a very long way in preventing problems later.
If you want to maintain a constant or minimum wall thickness in that area , some dimensions of the model need to be calculated based on other dimensions. The fillets you are pointing out are fixed size and don't appear to adjust based on other dimensoins. Aa such I did not see how you adjust the wall thickness.
It also is somewhat irrelevant to what I was going to demonstrate, because it makes no difference to to the end result where you dimension that fillet. 3.25 mm is ging to result in the same fillet regardless if you sketch it or apply it as a solid modeling feature. If the size of the fillet needs to be calculated it can be done in a sketch or in a solid modeling feature.
Also, of course there are instances where it is helpful and beneficial to apply a fillet in a sketch. I do that as well. The key here is to simplify the sketch where possible for the reasons stated above.
SUCCESS!!! I did it. Your method was perfect! Everything is correctly constrained and any adjustments to the various features causes everything to adjust itself accordingly, and thus is fully parametric.
Thanks again!
