Creating an external 'mould' from a solid

[Anonymous]

Hi all,

I've got a multi-part solid which I was originally planning on printing out, and wrapping in fibreglass to make a two part mould. However, I figured, why go to the bother... It should be easy to print the mould which will be the relief of the original part. I need some guidance on how to achieve this though. What I'm after is basically a 1cm thick layer around the external boundary of the part.

Part is available here.

Attached is an example, credited to Carbon Wasp cycles.

[johnsonshiue]

Hi! Although Inventor Mold Add-In was not designed for 3D Printing originally, it may help this case actually. Start up Inventor. Template -> Mold Design -> create a new Mold Design assembly. The environment should be fairly user-friendly. Autodesk Knowledge Network and the forum should provide good guidance.

Many thanks!

[karthur1]

Take a look at this.  Open the "Mold Cavity" part. It doesn't have the 2mm shell around the outside like you asked for,  but this is "one" way to do a mold cavity.

If you have any questions about what I did, post back.

Kirk

[Anonymous]

Thanks, that's a good option to fall back on. I can trim down the excess mould. To create a closer mould, in principle, would I need to build sketches from the profiles of the original part using project edges for the inside of the cavity and then my own additional sketch for the outside of the mould? Thinking ahead, I'll be able to build reinforcing ribs and flanges where the mould junctions with this approach...

[WHolzwarth]

Hmm. I've seen, that the bike frame is not symmetrical. Is that intended?

[Anonymous]

Ah yes, I see what you mean - I hadn't noticed that. I'll look into it. Good spot.

[Anonymous]

Now you've spotted that it's thrown a slight spanner into a loft. I found the missing dimension but a loft further down the chain isn't forming symmetrically - can you advise how I get loft 12 to form symmetrically?

[WHolzwarth]

Right now I'm looking closer at the shelled model. IMO, some changes are necessary.

I'll come back later.

[JDMather]

I found a large number of missing dimensions.

You can avoid these issues by fully constraining your sketches.

But this is fairly trivial to fix (without adding any dimensions) if you simply Project the XY plane into sketch Mid down tube and constrain the intersection of the two lines to the projected line.

Are you familiar with manual editing of automatic point mapping in Loft?

[WHolzwarth]

Meanwhile I've spent some time with this frame. Shelling it for carbon fiber purposes shows lots of problems.

I'm giving up

[johnsonshiue]

Hi! JD is right. Automatic mapping may not recognize symmetry. Unchecking the option will help. But, you still need to check each point map set to ensure they are mapped properly. For this particular case, you want to look at Set 4 and Set 8. Make sure they both snap to the mid point on the edge.

I see quite a few Sculpt features created by non-associative surface bodies. I assume you probably used Copy Object to get the surfaces. This will work only if the source faces will not be changed down the road. Instead of using Copy Object, you should consider using Thicken/Offset and set offset distance to 0. In this way, the surface bodies will be associative to the source faces. When the faces change, the zero offset surfaces will update and Sculpt features will update too.

Many thanks!

[Anonymous]

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@Anonymous wrote:

I found a large number of missing dimensions.

You can avoid these issues by fully constraining your sketches.

But this is fairly trivial to fix (without adding any dimensions) if you simply Project the XY plane into sketch Mid down tube and constrain the intersection of the two lines to the projected line.

Are you familiar with manual editing of automatic point mapping in Loft?

---

Ah yes, that's fixed the loft. I'm not familiar with manual editing of points, but now I know it's a thing, I'll look into it. It sounds like something that will be very useful. 

I'm still very much amateur at Inventor and I know I allow myself to take shortcuts on the sketches by not always fully constraining them. It's a habit I must break...

[Anonymous]

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@WHolzwarth wrote:

Meanwhile I've spent some time with this frame. Shelling it for carbon fiber purposes shows lots of problems.

I'm giving up

---

What process were you attempting to apply to it? The part is already shelled for FEA purposes, roughly demonstrating wall thickness. I'm wondering if you are attempting to shell the model in the opposite direction to create the mould with the frame as a cavity, not a solid? Thanks for looking into the query, I'll keep developing the design until it's right. I've plenty to learn and habits to break!

[Anonymous]

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@johnsonshiue wrote:

Hi! JD is right. Automatic mapping may not recognize symmetry. Unchecking the option will help. But, you still need to check each point map set to ensure they are mapped properly. For this particular case, you want to look at Set 4 and Set 8. Make sure they both snap to the mid point on the edge.

I see quite a few Sculpt features created by non-associative surface bodies. I assume you probably used Copy Object to get the surfaces. This will work only if the source faces will not be changed down the road. Instead of using Copy Object, you should consider using Thicken/Offset and set offset distance to 0. In this way, the surface bodies will be associative to the source faces. When the faces change, the zero offset surfaces will update and Sculpt features will update too.

Many thanks!

---

Yes, I followed some tutorials (not autodesk ones) that showed the process of copying object and using it to subtract from another object. I can see the problem with this method that you've raised - any future detailing of the frame will mean the sculpts no longer represent the physical part... I suppose I assumed that the copied objects were automatically associative. I haven't used the thicken/offset option. Can you link to a tutorial showing this process? I'll go back through the design and make these changes, along with revisiting the sketches and defining them properly. 

[johnsonshiue]

Hi! Copy Object can be associative when you do it between two parts within an assembly. Within the same part, Copy Object is not associative (associative checkbox is grayed out).

Thicken/Offset is relatively straightforward. The issue here is that you need to create an offset surface with offset distance = 0. I wish we had a separate command to copy faces as a surface body and then stay associative to the source faces. Here is a link to Thicken/Offset dialog. It should not be too hard to use.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2015...

Many thanks!

[JDMather]

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@Anonymous wrote:

I know I allow myself to take shortcuts .... It's a habit I must break...

---

In my experience, shortcuts frequently turn out to not be shortcuts.

[Anonymous]

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@johnsonshiue wrote:

Hi! Although Inventor Mold Add-In was not designed for 3D Printing originally, it may help this case actually. Start up Inventor. Template -> Mold Design -> create a new Mold Design assembly. The environment should be fairly user-friendly. Autodesk Knowledge Network and the forum should provide good guidance.

Many thanks!

---

Hi,

I've had a browse through the mould designer environment, and it looks like I'm going to end up with a large amount of material to print in building the mould, similar to Karthur1's suggestion. My aim in the mould is to keep excess material to a minimum by having the mould follow the shape of the body closely. If my current approach is no good, I'll investigate the mould designer further.

Using thicken surfaces, I've almost fully modelled the mould. However, I'm getting a lot of resistance from inventor with dialogue reports stating 'unable to perform bolean / remove faces / large topology change...' Sometimes by combining various faces or thickening one at a time I can make a little more progress, but I am discovering faces that simply wont thicken once others have been, and that I am required to try a loft between thickened faces to fill in the gaps (which also doesn't always work). However, this file is 80% what I want it to be, short of a few internal things to resolve. Can I get some assistance on discovering what is stopping the final few surfaces from thickening?

On a side note, I've revisited the sketches and it should now be fully defined.

[WHolzwarth]

Your basic solid has tiny gaps. Look at the yellow region.

This needs to be cleaned up before trying a thickening.

[Anonymous]

Thanks very much for looking - but I've no idea how you could tell where the problem is... I've done some inspection of the model and I don't see anything, and because that whole area is just a loft, I'm not sure where the gaps would be.