Different way to Create a Thicken/Offset Face?

[Anonymous]

I've got a question about the thicken/offset tool and wanted to see if anyone has any ideas to help out.  To put some context into this as well, I primary use Inventor to design for large format additive manufacturing.  I often design to oversize the parts because we are doing some secondary finishing of the parts.  I often use thicken/offset to enlarge the parts but this doesn't always give the result I'm looking for.

Its my understanding that the thicken/offset tool creates a new surface that is a set distance normal to the surface being offset.  By normal, I mean perpendicular to the surface in all 3 axis directions.  I would like to do an offset that that is only normal to the surface on cross sectional planes that are normal to a selected axis.  To do this manually, I  could create a loft from multiple offset cross section sketches but this can take a significant amount of time and can be very tedious when dealing with certain geometries.    

For example, in the attached model I have a half dome shape that has a 36in radius.  I can easily create a thicken/offset surface from the dome that is 2in inside of the current surface but this is not what I need.  To get what I'm looking for I can manually create planes, then sketches on each plane and project cut edges, then offset those lines, then use those lines to create a loft of the new dome.  This isn't perfect but with enough planes and sketches it can be very close to the original surface.      

Does anyone one have any ideas on how I could accomplish this in an automated fashion?  Could I use the existing in a different way to do this?  If it needs to be created manually, I'd like this to work on any geometry and have a selectable level of detail for the number of planes to create (or the distance between them), the offset desired for each sketch and the normal axis to use.   

I've already considered using shell but it creates the new surface the same way thicken/offset does.  I have also thought to copy and move a surface unidirectionally, to create the offset, but this is very limited in the geometry it can be used for. 

I've attached some pictures as examples and a model for reference.          

[Anonymous]

Here are a few pictures to better explain the concept.

[Justin.B.]

You could construct them the same way you construct your base geometry.

For this example I simply made another curve set to an equal radius as your first one, but with its center shifted 2 units to the side. This keeps a uniform width across the horizontal dimension at all points.

[blair]

When we design cast parts that require machining. We design the finished part first, then use the Derive function to create the "raw casting". We then use the "add" material either with the extrude command or the "Direct Edit" command. 

This way the raw casting is controlled by the finished part. We keep the link active, should something change on the finished part. 

[Anonymous]

Justin,

This does work in the specific example example of the revolved dome example I created but I often work with less symmetrical geometry that your method could not be used on.  I'd like this to be a generic method for any geometry. Thanks for taking a look.   

[Anonymous]

blair,

Your on the right path by thinking "raw casting" vs "finished part".  I checked out the options in the direct edit command and the "size" function looked promising but it still uses the same logic as the thicken/offset command. 

In my case, I'm looking get to a geometry that has a constant cross sectional thickness when looking on any plane along the specified axis.  For 3d printing this would be the z-axis so that the layers all have the same cross sectional thickness, which I need to optimize the printing process.  In other words, I need to print the "raw casting" model with a constant cross sectional wall thickness as opposed to a constant thickness wall.    

[arron.craig]

The only thing I can think of is to try out the direct edit scale tool and change it to non uniform and just leave the Z scale at 0.

You might be able to setup a scale factor parameter based on extrusion width with a bit of fiddling. 

[Anonymous]

Aaron,

That's an interesting idea and I think it could on axisymmetric geometries but not in general.  I looked at the dome example and applied a 0.90 scale to only the x and y directions.  Applying a single scaling factor won't work when a constant crosssectional thickness is needed.  The picture below shows the scaled down solid and the original surface.  The offsets at the top and bottom are not equal which makes sense with a single scaling factor applied to different dimensions.  

[Anonymous]

Does anyone have any suggestions on ways to automate the creation of planes, sketches, cut projections, offsets and a loft?

[johnsonshiue]

Hi Doug,

I took a quick look at the file you attached. I cannot seem to understand the need to create the Loft surface based on sections of the inner offset surface. Couldn't you just use the inner offset surface? What is the purpose of the loft?

Many thanks!

[Anonymous]

Johnson,

Thanks for taking a look.  The purpose of the loft is to create an inner wall that provides a constant cross sectional thickness when measured from the sketches on each plane in the example.  This is important for additive manufacturing because when the part is sliced by the software that creates the machine code, the wall thickness of the part will be consistent which makes for more efficient code.  The planes in the example model represent the slices. 

When you thicken/offset the surface the cross sectional thickness on each plane changes and gets thicker as the angle of the face relative to the plane increases.  This is why thicken/offset can't be used.    

[Justin.B.]

Your slicer should already be handling wall thickness. Instead of hollowing out your dome example in Inventor, you could just as easily set the full dome to have no infill and get uniform walls as a multiple of your extrusion width in your slicer.

Can you post an actual workflow example of what you're trying to achieve?

[Anonymous]

Justin,

Your right the slicer will do this but I also want to design in my own "infill" pattern.  I've modified the dome example by hollowing it out with my lofted surface and then added a single rib running through the middle.  The rib would be my "infill" and I could control the number, angle, position, etc. of the ribs through the design.   In my situation I only want to print using perimeters, and I also don't have the option for variable extrusion width in the slicer.  Given this, if I was to use thicken/offset or shell to hollow out the dome, the cross sectional wall thickness would be greater at the dome surface, which would leave a gap in the perimeters of the printed part.  Some slicers attempt to fill this gap with infill or "single extrusion infill" but I want to avoid theses extra extruder movements while still completely filling these walls. 

So this means I need to create a design with a consistent cross sectional thickness and my own design for the rib infill.  The most difficult part of this is creating the inner walls so that the cross sectional thickness is consistent.  I'm still looking for an automated way to do the manual process I've described (planes>sketches>cut edges>offsets>loft) if anyone has any ideas.

[johnsonshiue]

Hi Doug,

Many thanks for sharing the information! I think I got it now. The so-called offset distance (or wall thickness) is not measured at the surface normal. Instead, it is on a per layer basis for printing purpose. At the moment, Inventor does not have a good workflow to create such offset surface. As a result, you have to use Loft to approximate it.

Thanks again!

[johnsonri]

@Anonymous Here is a different way to go about it.  I attached the .ipt for you to roll back through the steps.  Curious to hear your thoughts.

Cheers

[johnsonri · Accepted solution]

Revised attached ipt for a simpler workflow. 

[Anonymous]

@johnsonri  I'm very interested in what you done but unfortunately I no longer have access to inventor.  Is there any way you could just post screenshots with a description?  I'm still searching for a solution but have yet to find one in any modeling software.

[johnsonri]

@Anonymous Here are a few screenshots to demonstrate.

1. You will need a sketch profile, in this case its a single line at the bottom that is 0.125" long.  This represents my desired horizontal wall thickness. You will use the sweep command with surface not a solid. 

        a. Then you select the 0.125" line as the profile.

        b. Then select the path which is your desired contour.

        c.  Select parallel and hit ok.

        d. Now you can see it created a surface with correct horizontal offset.

2.  Now you can revolve that surface as a solid around a central axis.

Let me know if this helps!

Thanks,

Rick

[Anonymous]

@johnsonriThanks! This looks like a pretty nice solution.  I hadn't thought of sweep and rarely have sweep a surface.  This will work for axis symmetric geometry and geometry with a single profile but if there is a surface with multiple curves it won't work.  Either way this is a good idea!