Getting an odd ripple, and I cannot find out what is causing it..?
Anyone up-to-date with 'SW isanity clause' to find out why something randomly does stuff?
Sorry John, that was tongue-in-cheek
Bare with me, didn't have all my morning coffee yet...
Morning Joe,.. I mean, John.... c'mon dude.. I need my coffee too!
You're trying to do far too much in one feature. Also, use the symmetry of the part to save yourself some work.
The bottom ends (in the orientation of your image above) seems to have a flat end plane. And don't try and model in what are essentially fillets, it's easier to create and edge to fillet afterwards.
Sorry Bjorn. I do not understnad what you're saying.
I cut the bottom edge becuase if I don't, the thicken is perpendicular to the plane, and ends up not being square to the top plane.
I think it has something to do with this yellow line that runs through the whole thing. I have another model which is doing the same thing in the area where I am having problems.
Hi Martin, what I mean is that the surface loft is trying to create too much at once, making it difficult to control the quality of the surface. Do it in sections.
The problem lies with the connecting lines. They are not user friendly.
I do not think this is a complicated curve feature. I have done much harder in the past.
I need to know how to manipulate the connecting lines properly. They seem to move at random, and then sometimes it cannot loft at all. It's like quantum mechanics or witchcraft!
Martin... Bjorn Hulman is saying all the right things.. there is too much going on with the curves and it would be better to do 1/2 and mirror (symmetry). image attached,.. there is a lot of distortion.. so.. it needs some more cleanup..
In this situation, I would suggest you use a Boundary Surface instead of a Loft, It provides much smoother geometry. To do this, select the long profiles for one direction (Selection Manager will be required), and then the cross profiles for the other direction. I think you need to add an intermediate cross profile at the place where the 'kink' is. Do this by using a spline on a new plane.
I did notice there was a minor issue with your initial 3D sketch. Not all the entities are tangential, therefore creating the ripple effect.
I would also be inclined to add thickness to the surfaces by using a mixture of offset surfaces and planar surfaces, instead of using the Thicken tool. Use the Mutual trim tool once you have done this to ensure that you have the required volume. you can knit these surfaces together to make a solid afterwards. Once you have the solid you can continue and create the features that you made before.
I have attached my attempt at the surfacing part. Hope this is what you were looking for!
Oliver,.. agree, boundary plays nicer and curves need more tweaking,.. although, if you turn on the curvature.. the offset (btw, you could have just thickened?)..it gets pretty turbulent.
How on earth do you use surfaces on a daily basis?? I find there are more reasons why this programme can't do something, that actually doing something.
Can't extrude this, can't thicken that, sketches keep disappearing, bulges suddenly appear when nothing has changed, cannot control connecting lines properly, can't merge, can't trim...
Thanks for the model by the way.
However, it still isn't what I am looking for, and doesn't expliain why the original ripple was there, nor how to resolve it directly.
Surfacing is a fairly complex tool, that requires practice and a good understanding of end/boundary conditions and which tools to use where. However really good results can be obtained from surfacing.
I think the ripple is caused in part because the entities in the 3D Sketch that is governing the whole model are not tangential (see image), hence there is a kink in the model. Also the thicken feature, much like surface offset will thicken that distance exactly normal to the face at every point. In this model as there is a small kink in the original surface which is exaggerated by the thicken feature. Turn on Zebra Stripes and Curvature in Evaluate to see the original kink when the model is rolled back to Surface-Loft4.
On a further note, when using Loft, you can only set End Constraints (i.e. normal to profile). Using Boundary Surface can create a much smoother surfaces as you can create constraints on intermediate profiles as well. You can also set constraints on the guide curves.
I agree with Bjorn that is is better to do this sort of surfacing feature in a number of features. Therefore you can create tangency to existing surfaces therefore making the whole model smoother. I think you need at least one or 2 intermediate profiles to avoid the kink as the two end profiles are considerably different.
I understand that it is complex, but I literally just tried to thicken something - comuter says, no! Went away from my computer, came back, and it worked.
It's a real head scratcher... If nothing is consistant, how can I amend and trust the difference..?
Martin,..well, here are a couple of ways.. and I'm sure it can be improved.. btw,.. don't know what the intent is or how bottom (mid/spine) blends.. so, I show a flat bottom and curved.
This model, and mine, end up having some sharp creases in them.
If I get this 3D printed, will those creases/lines be so dominant?
Still, thanks for the different models. Gives me a chance to try different approaches. I think I get what you guys are all saying now.
Martin,.. if you can add a radii at the sharp corner (~R20 applied to Sketch17).. it would help... you'd also need to split the face below to help it blend..
Thanks for that. I shall give it a whirl.
Now, I've just changed a 'Direction 1' sketch, now it keeps saying **error**, without any information when I try to add it...
I have two sketch on the edges, both identical. One works, the other doesn't
Any ideas what on earth it could be?
Make sure there are pierce relationships between your new sketch and all the DIR2 Sketches? Also see if changing the Boundary condition to Normal To Profile helps?
Believe it or not, if I select all sketches and try again from a different side, a different sketch (which was fine before) becomes an error sketch..?
Turns out it was an ordinal thing. If you select a sketch out of order, it just get confused. The **error**, technically shouldn't be an error. It just flags up as one i.e. SW cannot use the sketch in the order selected. When you use them in the right order, all is fine.
Some some reason, you cannot change the order of the sketched when they are selected. You have to deselect, the reselet them..? Odd, but true.
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