Why does 'surface output' become unselectable in extrude function?

[Anonymous]

Hi all,

I have two concentric circles that I have been extruding with a solid output into a hollow cylinder. I'm 'upgrading' my model from a solid to a surface but this is giving me a sticking point because I need all of the surfaces of the cylinder to be present. But I cannot edit the extrusion from a solid output to a surface output. I'm assuming that it is because it is two concentric circles... but why is this a problem and how can I obtain the faces (both external, internal and the two edges) without having access to an extrude to surface?

Thanks,

OLC

[swalton · Accepted solution]

Based on a quick test, Inventor only allows the user to select a solid or surface extrusion at creation.  The user can't go back and change from one to another.

Using Inventor 2018, I had to delete the extrusion feature, but not the underlying sketch to change from a solid extrusion to a surface extrusion or back.  Also, I was only able to extrude one circle at a time as a surface.  I had to share the concentric circle sketch and use two surface extrudes.

If you have already extruded the solid, you might try using the Delete Face tool without the heal option to remove the two ends.  That should give you an inner and an outer surface without having to delete the existing solid extrusion. 

Edit: Are you looking for all 4 faces (inner diameter, outer diameter, both ends)?  If so, try the patch command to create the two end surfaces.

[johnsonshiue]

Hi! There isn't a real technical reason for the behavior. Certainly, it could be technically more challenging to allow body type to change from solid to surface. But, it is doable. It is more like a design choice. Most of the workflows in Inventor are geared toward creating solid bodies. The potential of surface modeling is not yet fully unleashed. I think there is room for improvement here.

In the meantime, could you tell me why you want to change the solid body to surface body? Do you need the cylindrical surfaces? There are two workflows to do that easily.

1) If you no longer want the solid to stay as solid. you can simply use Delete Face command to delete the two planar faces on each side. You will get the deleted face body, which is actually a surface body.

2) If you still want to keep the solid body, you can use Offset command, select the cylindrical face, and set the distance to zero. You will get a separate surface body on top of the cylindrical face.

Many thanks!

[Anonymous]

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@swalton wrote:

Based on a quick test, Inventor only allows the user to select a solid or surface extrusion at creation.  The user can't go back and change from one to another.

Using Inventor 2018, I had to delete the extrusion feature, but not the underlying sketch to change from a solid extrusion to a surface extrusion or back.  Also, I was only able to extrude one circle at a time as a surface.  I had to share the concentric circle sketch and use two surface extrudes.

If you have already extruded the solid, you might try using the Delete Face tool without the heal option to remove the two ends.  That should give you an inner and an outer surface without having to delete the existing solid extrusion. 

Edit: Are you looking for all 4 faces (inner diameter, outer diameter, both ends)?  If so, try the patch command to create the two end surfaces.

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Thanks, this was very informative. I got a bit stuck in a cycle of selecting my extrusion to change from solid to surface and being greeted with the hurdle... And thinking why on earth wouldn't it... Having deleted the extrusion I can now extrude one circle at a time. I was hoping that selecting both would give me the same surfaces as the extruded body. My first look has been at joining the edges of the extruded circles to close the object into a cylinder. But I haven't worked that one out yet.

[Anonymous]

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@johnsonshiue wrote:

In the meantime, could you tell me why you want to change the solid body to surface body? Do you need the cylindrical surfaces? There are two workflows to do that easily.

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I'm working on bicycle designs so I'm working with tubes, not solids. Sketches define the outer surface profile of the tubes. Before I'd understood surfaces I'd been designing with solid lofts which is useless within the FEA module (though that is currently beyond my experience). But actually, my end goal is to have a female mould of the tubes, not the tubes themselves - using surfaces means I can easily change from a thickening that defines the tube wall thickness in one direction, to a thickening in the other direction which creates a mould of the tubes. I was having problems getting a mould of the tubes when I was using solids. My experience thus far tells me that for my purposes, surface modelling is actually more useful.

[johnsonshiue]

Hi! I understand it now. I agree with you that surface modeling is very powerful. I have been using it to solve various design challenges. Conceptually, solids and surfaces are the same. They are creating the shape. Surface modeling allows better intersection control. But, somehow most parametric solid modelers (Inventor included) were designed with solid modeling with higher priority.

Many thanks!

[swalton]

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@Anonymous wrote:

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@johnsonshiue wrote:

In the meantime, could you tell me why you want to change the solid body to surface body? Do you need the cylindrical surfaces? There are two workflows to do that easily.

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I'm working on bicycle designs so I'm working with tubes, not solids. Sketches define the outer surface profile of the tubes. Before I'd understood surfaces I'd been designing with solid lofts which is useless within the FEA module (though that is currently beyond my experience). But actually, my end goal is to have a female mould of the tubes, not the tubes themselves - using surfaces means I can easily change from a thickening that defines the tube wall thickness in one direction, to a thickening in the other direction which creates a mould of the tubes. I was having problems getting a mould of the tubes when I was using solids. My experience thus far tells me that for my purposes, surface modelling is actually more useful.

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As I understand it, the FEA module in Inventor Professional (not InCAD) needs a 3d solid as a starting point.  It can compress a "uniform" thickness solid into a surface to improve solution time, but it can't start with a surface.  

Have you looked at iParts?  You could make your tubes as iParts with two members.  One member with the thicken to the inside, the other to the outside.

Have you looked at the mold design tools in Inventor? These tools may be useful for your mold parts.  See: http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-B3CD4078-8480-41C3-9C88-C470E9AC686C

[JDMather]

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acjswan wrote:

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1. I'm working on bicycle designs so I'm working with tubes, not solids.

2.  Before I'd understood surfaces I'd been designing with solid lofts which is useless within the FEA module .... 

3. end goal is to have a female mould of the tubes, not the tubes themselves - using surfaces means I can easily change from a thickening that defines the tube wall thickness in one direction, to a thickening in the other direction which creates a mould of t....

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1. Every bicycle I have ever owned was solid.

2. I have never heard this before.  I use Lofted bodies in FEA all the time?

3. Mold Environment or Derived Component.