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Why can't I draw this?

Why can't I draw this?

I can change the radius to 1,9 or 2,1, than it is accepted, but 2 not. OK, the result in real live with a diameter of 2 won't be pretty, but with 3 neather.

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Solid Edge ST9 & AutoCAD 2018 user
14 REPLIES

Re: Why can't I draw this?

[ Edited ]

Simple - your holes are tangential to the top surface of the recess when the diameter is 2.

There are loads of threads on this message.

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Re: Why can't I draw this?

It's tangential, OK, so???

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Solid Edge ST9 & AutoCAD 2018 user

Re: Why can't I draw this?

Parasolid doesn't support 0 thickness walls (on a single body) so you got that error message.

As you said, in real life that can't exsist, the 0 thickness wall will broke during milling.

Re: Why can't I draw this?


Fiorini wrote:
the 0 thickness wall will broke during milling.

Right.

zero-thickness = non-manifold = non-manufacturable = not-allowed

Re: Why can't I draw this?

[ Edited ]

If that's the reason, a hole of 2.01 would be allowed neither...

Software should do what I ask, not what they think is wright.

 

I can shoot a wooden peace on this plywood, drill the 2mm hole and remove the wooden peace. So yes, I can drill a 2mm hole on 1mm from the side.

Nothing magic here...

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Solid Edge ST9 & AutoCAD 2018 user

Re: Why can't I draw this?


Joris wrote:...

Software should do what I ask, not what they think is wright.

...

This is a really common complaint in CAD. You hear this come around every couple of years on just about any CAD system. "Why can't we create zero thickness?"

 

Think of it as a limitation of solid modeling. Solid modeling is 3 dimensional and requires volume. A zero thickness condition reduces at least one dimension to 0. Math doesn't like 0.

 

So if you don't like the zero thickness error and you think you should be able to do it, you have some options: You can start making surface models that don't require a non-zero distance between faces, you can draw it in 2D, or maybe use a polygonal modeler that doesn't know anything about volume.

 

Is it possible to reconfigure Solid Edge so that it allows stuff like this? I suspect this is a Parasolid limitation, really, and certainly not exclusive to Edge. Could they do it? Probably, but then, and I don't know this for 100% sure, but this is what I believe, then you would be disabling so much error checking that you would find it hard to make sure that your model was even possible. You could run into situations where the outside of a part was actually smaller than the inside (it is easy to demonstrate SolidWorks doing this - essentially making a part where the inside pokes through the outside - specifically because they play fast and loose with error checking).

 

And that's not even addressing the question of manufacturability or good design practice.

 

It's a problem that even as a temporary state in an ordered model, a feature will fail if it creates zero thickness at any point in the feature tree. So you just create another feature first that eliminates the zero thickness. Or you make the difference small enough that it's below your manufacturing tolerance.

 

You just can't say "it should do whatever I tell it to do", that's just not realistic, especially if you don't understand why the error is necessary in the first place. Be careful of what you ask for. This is one of those things that we have to work with in order to get the rest of the benefits of solid modeling.

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Re: Why can't I draw this?

As Matt mentioned non-manifold conditon cannot exist because the math on the volume cannot be calculated. To say zero-thickness is not supported is incorrect because surfaces are actually all zero-thickness entities.

 

The real problem for the CAD software is to determine the vector normal for the edges of the 3d solid. Since you have two edges that share a common edge the vectors point in opposite directions for the same edge. You can't have two vecotrs define the surface normal in a surface definition. That is what causes the problem.

 

I had to chuckle at the SW users this years as they voted for the enhancement requests and voted for allowing this condition to occur. It was explained that this was driven by the Parasolid modeling kernel (owned by Siemens PLM) and that they would probably not allow this change for the many reasons Matt mentions. But they wasted thier votes anyway. I guess some engineers and designers don't get the concept of an accurate "solid body" instead of an approximate body! ;-)

Re: Why can't I draw this?

Ryan: (The real problem for the CAD software is to determine the vector normal for the edges of the 3d solid. Since you have two edges that share a common edge the vectors point in opposite directions for the same edge. You can't have two vecotrs define the surface normal in a surface definition. That is what causes the problem.)

 

Wrong Ryan!

One can have a common edge for the 2 surfaces and Parasolids is not quiting on us and part is 'not manufacturable' then.

 

See the sample.

I have there two vectors in opposite direction defining the surface normal in a surface definition.

 

What if one needs/wants to define 3D geometry with the common edge in the middle of 3D definition process and than places later fillets or something similar on that edge.

 

Milan

Re: Why can't I draw this?

[ Edited ]

Except in that example @milanw, the vectors know their convergent endpoints....try the same thing, with the rounds extended further, it makes the point.

 

[if you edit the profile of the attached "modified" ST8 file, you'll see what I changed]

 

EDIT: images added here for clarity to others, not on ST8.....

 

[Milan's part profile]

 

[my modified version]

Sean Cresswell
Design Manager Streetscape Limited
Solid Edge ST10 [MP0] Classic [x2 seats]
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