can not thickness this helmet@@

[emills2]

Double-clic an edge in the list.

thanks Chris, i would never have guessed it. Making some progress. my 'cross' of guides on top is a bit bit too much and makes the surface wobble when i set G1 (but the G1 to the extrusion is clean).

right now i'm frozen because i rebuilt and set G1 before setting the upper guide....i'll gt the right selection order eventually.

[emills2]

finally. this is what i came to FreeCAD for after finding out about the existence of OpenCascade! it only took 15 years to reach the GUI

putting in all the guides i had earlier made it lumpy. but eliminating the cross, and making the top guide a single curve finally did it. (split top guide wouldn't make a surface)

the side profiles don't even need to be split anymore, because we don't have to line anything up in that direction. It's handy as split if you want to dimension the width exactly.

order of operations:
-select the boundary curves (as edges of the extrusion surface, hide the sketch splines)
-leave the face/continuity business ALONE for now
-add the top guide under unbound edges
-now go back to the boundary edges, double click, select the one face available, then G1 (not G2, it would conflict with our guide)

tadaa! it's a new era of FreeCAD starting for me not sure who exposed all the options of OCC surface filling, but thank you.

Helmet_02_01.PNG (287.07 KiB) Viewed 981 times

what would really be nice is point on spline in the sketcher. it could be strictly driven (if that helps solving the spline), then we could link sketches downstream without splitting splines in sketches.

maybe point on external spline would work? it cause no recomputation of the spline and its constraints.

[emills2]

and another problem, how i make it solid^^??

surface tool, flat cap on the bottom. Part > Shape Builder, shell from faces. then solid from shell. then thickness to hollow it out

from your picture, it looks a little 'lumpy'. make sure that's ok before going too far.

[ethan0124]

this my file:
https://drive.google.com/open?id=190xpQ ... dHsmL4_Gd2

when i do thickness in part workbench, it was fail all the time, i do not know how to deal with it........><


plz help me!!

[emills2]

can't look at your file right now, but i'll bet a donut it's the lumps i mentioned. you might think it's only esthetic and doesn't matter, but lumpy pinched surfaces cannot be worked on down the line.

that's assuming you successfully created a shell and a solid.

i think this topic would be nice to keep with the other thread. longer thread to read, but more complete. i can't reply to two threads and PMs at the same time.

i'll try to help later if you agree to keep posting in the original thread and let this one die.

[chrisb]

I merged both topics.

[chrisb]

Thickness is a very picky operation and it often fails if the geometry becomes complicated. I guess that the surface kills it.

[oldmachine]

It's true that 'Thickness' is fussy... But, there are some things that can help...

The image below shows a surface made from two-curves.
Adding a Cube to encase that completed surface, then doing a Boolean, produces a result that can be converted to a Solid.

Trying to hollow-out the solid with the 'thickness' tool will not work because of sharp edges (though you don't know that).

To tweak it so it will hollow-out, adding a Fillet to the edges removes the problem, as shown below...

[ADDED the File]

[emills2]

this my file:
https://drive.google.com/open?id=190xpQ ... dHsmL4_Gd2

when i do thickness in part workbench, it was fail all the time, i do not know how to deal with it........><


plz help me!!

ok, i finally have time to look at this.

It looks like you adapted my sketch layouts and redid the splines as arcs. you used the same type of data in your fill surface, edges from the extrusion of the flat profile, and one 'rib' running front to back. You obtained a very good looking surface fill. no lumps.

When i saw that, i thought oldmachine must be right, the sharp corner in the front might be causing problems.

However, before trying that, i decided to check your solid (from the surface shell) by applying thickness directly:
it fails no matter what!

Helmet_thickness_00.PNG (128.13 KiB) Viewed 911 times

the extrusion and your file in general does seem sound

Helmet_thickness_01.PNG (138.34 KiB) Viewed 911 times

so it seems it doesn't like your surface controlled by arcs. i don't know why yet.

before digging into that, i decided to try thickness on my model. my model has 2 splines on each profile half (could be just one, no specific midpoint is really needed here), and one spline for the front to back top 'rib'. so i added the bottom face, shell, solid, thickness.

it works:

Helmet_03_00.PNG (270.25 KiB) Viewed 911 times

i included the model file. i invite you to play with it while i try to find a fixable reason why your joined arc profiles don't work.

i usually prefer splines over arcs, but there will be times arc profiles are needed, so it's worth investigating. if you want to do product design type stuff, splines and NURBS will need to be part of your skill eventually. So you will gain a lot from learning them anyways.

EDIT: i don't even know how to use half of the features in the Sketcher NURBS, and i don't bother, because i made my own 'baby NURBS' workbench:
https://edwardvmills.github.io/Silk/ it doesn't allow as many points, or changing the knot vector, or the degree, but allows me to control the crap out of a 4 point cubic bezier curve!

[emills2]

anomaly detected: DESTROY!!!

in this sketch, everything appears symmetric and tangent constrained....but then why are all the arc center points NOT symmetric?

Helmet_thickness_02.PNG (87.35 KiB) Viewed 909 times

this is the kind of situation that could create virtually undetectable LUMPS!

The surface tool output looks good, but it could have tiny wobbles that make the surface impossible to project, because offsetting amplifies the wobbles! f you can't create a clean offset surface, you can't build a thickness.

it's a fun theory...i'm going to try it out. i'll delete some dimensions and try to pin some arc centers to the y -axis