Problem while smoothing

3D Design
1

Hello

I want to create a smoothing between two sketches but unfortunately, it doesn't go the way I would like. After smoothing, one of the corners or one of my faces deforms (Illustration with the image). During the smoothing, I select one of the sides of the 1st sketch and then one of the sides of the 2nd. I tried with different lines and dots, always one of the corners that doesn't follow the movement.

When I select the sketches in the work tree, I get an error message: construction error.  

Finally I tried to create a guide curve connecting the two sketches in order to overcome the problem, but without result. 

If someone could explain to me the problem and what I'm doing wrong..  

Thanks in advance


erreur_de_lissage.pdf
2

Hello rd_6

Could you make an image or a PDF of your sketch(es) as well as the guide curve(s).
Do you use "swept base" or "smoothed base".

In addition your part (sheet metal) has a high draft but it would not have the same angle depending on the place, if I can see correctly.

Like that  at first glance I would say a flaw in the sketch. The angle in question must not be made in one piece but with two pieces of curve or a straight end and a curve.

Kind regards

1 Like
3

I will send you the requested files. 

Sketch 1 which is on the xy plane is made at z=0. Sketch 2 is also on the xy plane, but with a z=450mm. The 1st part of sketch 1, back (which is straight) is projected onto sketch 2. And the front of sketch 1 is offset by 180mm keeping the same shape in order to have this draft.

I use smooth base, because swept base the back part that should be straight is not. It follows the guide curve. 


esquisse.pdf
4

I think there are 2 solutions to the given problem

1) multiply the guide curves in line with the angles, one at each end 

2) create the basic sketches with sharp angles and then radiate obviously in a solid body and finish with a shell function

@+;-)

5

Hello

1- No need to do the whole outline: only do half if it's symmetrical. This generates less error sometimes when smoothing.

2- Can you post your file, because there is no problem with 1/2 sketch or complete sketch. ?


2020-03-20__esquisse_2.pdf
1 Like
6

Hello

I just remade an equivalent part and after correction I no longer have a problem:

For a smoothing there is one thing that avoids deformation is to have the same number of knots on the bottom and top part, except when you created your 180 offset at the front you added 2 strokes to extend but it creates 2 more knots. (red arrows)

To fix this, remove the V or A part:p Pull the sides forward, create your offset of the V-part to 180mm without the fillets and connect with the sides.

Add the fillet then make your own smoothing without a guide curve.


lissage.png
7

@opiep you have unintentionally corrected the problem in your example by merging the sides.;)

8

Thank you all for your answers. 

@FUZ3D Thank you for your answer which will prevent me from creating smoothing errors from now on