Creating a solid

[whitakerp]

I am creating a fuselage for a helicopter. The facility that will manufacture them has responded with the following statement. Could someone explain what it means? Is there a way to convert from a shaded to a solid version? The file is attached.

'The problem is the part in step drawing is not complete, only have some surface. Do you have the complete drawing with solid, not only surface?'

Many thanks,

Patrick

[helo10]

Hi Patrick,

Could someone explain what it means?

'The problem is the part in step drawing is not complete, only have some surface. Do you have the complete drawing with solid, not only surface?'

Can try.. : The step file you sent them did not contain a solid like a box or so, instead there were only surfaces ( for example 3 face of an box ).

Is there a way to convert from a shaded to a solid version?

shaded? did you mean surface? In Part Workbench there are tools to create a solid from an surface/shell if the surface is closed.

But I think the problem is somewhere else:
You created some solids to get your fuselage but you did not use boolean operations to fuse them. So you have a couple of solids which intersects. I do not know how you want to get the fusealge manufactured (maybe you could give some more information), but I would guess that you need one solid.

How did you export to the step file? Could you post the step file as well?

btw instead of 4 chamfers at the top you could have used 1, selecting all edges

[normandc]

If Patrick selected all the solids for STEP export, it's possible the resulting shape wasn't "watertight". There are conflicting inner surfaces that prevent correct fusion. For example the rear fin block has 4 slots going through it sideways. When you try to fuse the fin block with the body fuselage, the fusion fails and loses the end ring of the fuselage. The sketch creating the fin will need to be changed to remove the slots. They need to be copied to another sketch then cut through with the pocket tool. Also having them through the shape is a bad idea. I would only cut the surface by some depth, each side of the fin block. Otherwise your mold maker will tell you it's impossible to make.

Also there are two copies of the fuselage visible. You need to take care to use only one copy for the fusion and hide the other.

I am very surprised the mold maker requested a simple solid. Is he going to take care of modifying it to have two half shells? Is it injection molding?

[whitakerp]

I guess that was the newbie question of the year. Here is a version with everything a solid except for the spheres. I don't seem to be able to upgrade them to a solid. There is an error message 'Upgrade failed'.

Many thanks for the help.

Patrick

[normandc]

What do you mean "I don't seem to be able to upgrade them to a solid"?

Did you use that tool? https://sourceforge.net/apps/mediawiki/ ... ft_Upgrade

That was not the right tool for the job. To combine solids you need to use Fuse from the Part workbench. https://sourceforge.net/apps/mediawiki/ ... =Part_Fuse

By using Draft Upgrade instead of Part Fuse you seem to have destroyed your history. The Shell object has no relation to any other object. Use Tools --> Dependency graph to see what I'm talking about.

In fact the Shell object seems to be a compound object (which groups multiple elements) and is neither a shell nor a solid. This prevents any boolean operation with other solids.

You have to start again, this time using boolean operations from the Part workbench, not Draft tools.

[normandc]

There's a problem with your Revolution feature. Activate the Part workbench, select the Revolution feature then go to Part --> Check geometry. Or in the toolbar, it's the blue cone with a magnifying glass over it.

You get this in the Task panel:


It's telling you the resulting shape is invalid because it is not closed. So I went to look in the Sketch under Revolution. On one end of the sketch, you have this:

(Never mind the fact the dimension text is mirrored, this seems to be a display bug)
Seemingly those two dimensions are identical at -2.23mm. Right? Wrong. If you double click on each one, you will get a dialog box allowing editing of the value, The dimension for the construction line endpoint reads -2.23475, but the dim for the vertical line endpoint reads -2.23497. This means the vertical line goes below the rotation axis. Even if it's by a minute amount this is bad, because it means it creates a self-intersecting surface, which prevents the creation of a "watertight" shell, thus preventing the creation of a valid solid.

At the other end we have the same problem, but over that, the vertical dim for the construction line endpoint is now -2.23332. It means that your construction line, which is used as rotation axis is not perfectly horizontal.

You did not listen to the advice I gave you in your other topic.

Some general tips: use as many geometric constraints as you can in opposition to dimension constraints. And dimension your sketch elements to each other, don't rely too much on dimensioning to the XY axes.

You should have used only one vertical dimension for your construction line, and a horizontal constraint.
You should use a point on object constraint for your vertical line's endpoint at left and arc endpoint at right of the sketch. Both to connect to the construction line. Then you ensure they are coincident to your rotation axis and that you get a valid solid.

Another thing: don't leave dimensions as they are at the time of creation. Double-click on them, and round them up. At least for straight elements (for arcs it's not as important as they are only aesthetic elements). CAD is precision work. Making sure to round your values will save you trouble later (like right now). I would have rounded that 2.23475 value to 2.23.

Finally, one thing about your rounded end. Your arc as it is right now does not create a true hemisphere.

[whitakerp]

I received this message from the production facility:

'FreeCAD software only can do the drawing without the solid. So when you save the drawing for other format, the drawing only have some surface.'

There were apparently errors in the .STP export. They installed FreeCAD to obtain a complete solid.

Thanks to everyone for the help with this, including the book.

Patrick