Drawing the Same Mold Using Fusion 360 and OnShape CAD

In progress and coming soon.
While running, with nothing open, Fusion 360 gobbles up 1.8gb memory and consumes 148 processor 148. Its program folder uses 10G bytes of disk space and contains 96,000 files. OnShape does not need installation because it runs in a browser tab that consumes one-fifth the amount of memory.


1
I am launching Fusion Three-Sixty to create a case-mold for a classic beer bottle shape.
After 3D-printing, it can be filled with plaster to create a working slip-casting mold for ceramics.
As you can see, Fusion takes a while to start up, even on a fast computer.
While we wait, let's start OnShape 3D from its login page online. I'll click the button now. Wow, that's amazing.

Back in Fusion Three-Sixty, here is a dialog I often get on startup. It costs about $750 per year and I can only use it on one computer at a time!
These things have really been testing my romance with this software lately.

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Let’s get started. I’ll make sure I am in the Solid workspace. I brought up the Parameters dialog from the Modify menu and am adding four parameters: Shoulder height, body radius, body height and plaster thickness.
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Now, let's go to OnShape and do the same thing.
First, I'll create a new drawing and open the Variable Table and add them in a similar manner.
It is more convenient here to enter the names first and then the values.
OnShape also makes it easy to create variables while dimensioning. We can learn that later.
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Create a sketch on the YZ plane.
Start a line from the origin, go left a little, type "13.5" and press the Enter key (while keeping the line horizontal). Notice Fusion has constrained it horizonta by inference. Go down about twice that distance and outward a little, click and then press the Escape key. Hide the data panel and zoom in if needed. Use the Dimension tool from the Create menu to dimension the bottom point from the origin: 15mm left and 36mm down. Finally, move the dimensions out of the way.
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Now, let's do the same in OnShape.
I'll hide the front and top planes and make a sketch on the right plane. I'll drag the viewcube using the right mouse button, then click on that face.
Using the line tool I'll draw two line segments from the origin as before. This works a little differently than Fusion.

I click, then enter the number 13.5, then press the Enter key. I'll click again and press Enter (because I don't know the linear length). Using the Dimension tool I'll set to bottom point 15mm left of the origin and 36mm vertically down. Like before, I'll move them out of the way.
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In Fusion Three-Sixty, I finished the sketch after the last step, so now I'll find it in the browser and edit it again.
I'll zoom out and then draw lines for the body vertical and base (it wants to constrain them to vertical and horizontal so I'll follow its lead) and then finish at the origin to form the center line.
Then, I'll constrain that center line to vertical.

Next, I am going to use the "point-tool" and create a point a little down and to the right of the bottom of the neck.

Finally, I'll round that bottom corner using the fillet-tool, I'll click on it, type "6" and press Enter.
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I am back in OnShape the next day. I had to sign back in and open this drawing.
Next, I'll right-click the sketch and choose "Edit", then hide the right plane.
Then draw lines for the body vertical and base.
And finish at the origin to form the center line.
Then I'll constrain them to vertical or horizontal (since that was not inferred while I was drawing).

Next, I am going to use the "point-tool" and create a point a little down and to the right of the bottom of the neck.

Finally, I'll round that bottom corner using the fillet-tool, I'll click on it, then off it, then type "6" and press Enter.
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Now, let’s do some dimensioning, starting in Fusion Three-Sixty.
First, the point. 5 mm down from the neck bottom and 12.5mm in from center. In each case I use the dimensioning tool, click on the items, type the amount and press the Enter key.

Next, the shoulder height, using the parameter already created. For these, I begin typing part of the parameter name and press Enter twice when it is the only one left in the list.

Next, the body radius, again using its parameter. But first, notice I can press the Escape key and move the bottom down. This is possible because that part is blue (meaning it is not yet defined) The "D" key then restores the dimension tool.

Then I'll dimension the body height, doing the same. In each case, the existing constraints enable choosing points, lines or both.

Finally, I’ll connect the neck and shoulder through the point using a spline (finishing with a double-click on the lower point).
And then tangent both ends manually.
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Let’s switch to OnShape and do the same. "D" is also the shortcut for the dimensioning tool.
Let's dimension the point 5 mm down from the neck bottom and 12.5mm in from center. Like Fusion, I click on the items (being careful not to move while doing so), then type the amount and press the Enter key.

Next the shoulder height, using the parameter already created. For parameters the procedure is the same as Fusion.

OnShape uses the same blue color to signal this part is undefined. As before, I can press the Escape key and move the bottom down. Then set the body radius using its parameter.

Then I'll dimension the body height, doing the same. In each case, the existing constraints enable choosing points, lines or both when dimensioning.

Finally, I’ll connect the neck and shoulder through the point using a spline (finishing with a double-click on the lower point).
And then tangent both ends manually.
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Back in Fusion, I'll add a natch hole 13.5mm in diameter.

And then fine-tune the shoulder contour by dragging the handle that controls the curve.

Then I'll use the line tool to start drawing the inner mold wall, starting at the bottom centre line.

I'll use the plasterThickness parameter to set the distance of the base from the bottom of the bottle.

I'll let it infer the horizontal base vertical wall and then angle up toward to top and join at its corner. Then I'll set that top line horizontal.

To finish, I'll bevel the bottom corner by 20mm.

And then constrain the shoulder points of the bottle and mold horizontal to each other.
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Let's do the same in OnShape. I'll add the 13.5mm natch hole by clicking, dragging, clicking, entering the number and pressing the Enter key.

And then press the Escape key and fine-tune the shoulder contour by dragging the curve handle.

Then, I'll use the line tool to start drawing the inside wall of the mold, starting at the bottom center line.

I'll let it infer the horizontal base and vertical walls and then angle up toward to top and join at its corner. Then I'll set that top line horizontal.

Next, I'll use the dimension tool to set the distance of the base from the bottom of the bottle to the plasterThickness parameter.

To finish I'll bevel the bottom corner by 20mm.

And then constrain the shoulder points of the bottle and mold horizontal to each other.
12
Back in Fusion Three-Sixty I am dimensioning the gap between the side wall of the mold and the bottle to the plaster thickness parameter.

And then the width of the top edge against the neck to 25mm.

Now, I'll reposition the natch.

Next, we need to draw the containment wall of the mold. Let's do that by offsetting the outer edge, all the way around, outward by 0.8mm.

We'll finish by closing in the two ends, being sure they are vertical.
At the bottom there is a little piece I need to remove, I'll do that using the scissor tool.

Finally, I'll finish the sketch.
13
Back in OnShape, I'll dimension the side wall gap, setting it to the plaster-thickness parameter.

And then the width of the top edge against the neck to 25mm.

And I'll reposition the natch.

To draw the containment wall of the mold I'll use the Offset tool also. I'll select the chain of lines all around the outside, move to offset outward, press the Enter key, then type in 0.8mm.

We'll finish by closing in the two ends, being sure they are vertical.

Finally, I'll finish the sketch.
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Back in Fusion, I'll pick the Extrude tool. I'll select everything except the natch hole. I'll type "-0.8" and press the Enter key.

The same technique works to extrude the walls upward. But, the sketch has been turned off.
I'll turn it back on. This time, I'll enter parameters: body radius plus plaster thickness.

I'll check to make sure the "join operation" is set and then confirm.

Finally, I'll use the "revolve tool" to revolve the bottle by 90 degrees, around the center axis, again using the "join operation".
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Back in OnShape, I'll pick the Extrude tool and the extrude dialog will appear.
I'll select everything except the natch hole. Begin dragging backwards to select the direction, and then set the depth at "0.8", and confirm by clicking the check mark.

The same technique works to extrude the walls upward. Like Fusion, the sketch was turned off. So I'll turn it back on.
This time, instead of entering a number, I'll enter parameters into the depth field: body radius plus plaster thickness.

I'll check to make sure the "add operation" is set, so this combines with the base already extruded, and then confirm.

Finally, I'll use the "revolve tool" to revolve the bottle by 90 degrees.
I'll select the bottle, then the axis, then set it to revolve in one direction, at 90 degrees, again using the "add operation", a finally, confirm.
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Back in Fusion Three-Sixty, I'll make a sketch, on the vertical face, to draw the lug.
I'll begin by creating a corner rectangle of 5x10mm.

And then make it vertical with the origin (not the bottom of the part I already extruded).

I'll dimension it to be 17mm down.

And then finish the sketch, turn it on, and extrude it 18mm through the bottle (using the join operation).
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Back in OnShape, let's do that same thing.
I'll make a sketch, on the vertical face and create a corner rectangle of 5x10mm.

And then make it vertical with the origin.

And dimension it to be 17mm down.

And then finish the sketch, and extrude it 18mm through the bottle (using the add operation).
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In Fusion Three-Sixty I'll choose the Draft-tool and then select top face of the lug as the pull direction.

It then wants me to select the draft-faces.
I'll choose all three.

Next, I'll set the angle at 30 degrees and finish.

Finally, I'll choose the Fillet-tool, then select the 8 concave and convex corners, set it to 2mm and finish.
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In OnShape I'll choose the Draft-tool and then select top face of the lug as the neutral plane.

It then wants me to select the entities to draft.
I'll choose all three.

Next, I'll set the angle at 30 degrees and finish.

Finally, I'll choose the Fillet-tool, then select the 8 concave and convex corners, set it to 2mm, and finish.
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Back in Fusion Three-Sixty, I'll select the Shell-tool. Then I'll select the two flat faces of the body of the bottle.

Then enter a wall thickness of 1.2mm and finish.

Next, I'll choose the Mirror tool and then select the mold.
I'll tell it I want to set the the mirror-plane, and do it.
Finally, I'll make sure the join-operation is set, and then finish.
21
In OnShape, I'll choose the Shell-tool. Then I'll select the two flat faces.

Then enter a wall thickness of 1.2mm and finish.

Next, I'll choose the Mirror tool and then select the mold.
And then the mirror-plane.
Finally, I'll make sure the add-operation is set, and then finish.
22
Back in Fusion Three-Sixty, I notice that I forgot to chamfer the inside bottom perimiter.
To do that I will first roll the timeline marker back one step.

Then choose the Chamfer-tool, select the inside corners, but not the top.

I'll set it at 4mm and finish.

When I move the timeline marker back to the end, the mirrored half will also have the chamfer.

Lastly, I'll edit the first sketch, and move the hole a little.
When I save it, that change will ripple all the way to the last step.
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In OnShape, I'll do the same.
I'll roll the timeline marker by right-clicking on the previous step.

Then choose the Chamfer-tool, select the inside corners.

I'll set it at 4mm and finish.

Then I'll roll back to the end.

Lastly, I'll edit the first sketch, and move the hole a little and save.
Like Fusion, the change ripples all the way to the last step.
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Now, let's admire what we just made.
In Fusion Three-Sixty, I'll choose the perspective camera and rotate the drawing.

Lets do the same in OnShape.
Here, I'll choose the isometric view.

I hope you are as amazed as I am that such a complex drawing can be done in so few simple steps.