Spirals

stephen_sjodin

Hi Folks,

I just started with Onshape yesterday.  Love it so far.  I'm an aspiring inventor not an engineer or CAD expert.  I'm finding Onshape to be really intuitive.

Now what I'm trying to do is recreate a scroll pump (see http://en.wikipedia.org/wiki/Scroll_compressor) that I did in FreeCad. I like FreeCad but my desktop is just not up to the task when things get complex... or maybe it's FreeCad that is limited, I'm not sure.  Nevertheless, FreeCad has these geometric primitives that I can use to define a spiral path to sweep on.  Is there something similar in Onshape (yet), or is there another way to do it?  

Here's the lower half of a pump I drew in FreeCad.



I saw a blurb about using a helix on a cone here:  https://forum.onshape.com/discussion/comment/5073/#Comment_5073 but I don't see how that would work for me.  The geometry of a spiral may be different and the top of it in this part would have to be flat.

Cheers

jakeramsley

Looks like you have a 2.5 turn spiral that is flat.  What I would do is create a cone that has the inner radius at top and the outer radius at bottom and attach a 2.5 turn helix to it.  Then sketch on a plane and project the helix.  This remove the z-depth and flattens it into a 2.5 turn spiral.  From here I would probably extrude the spiral as a sheet, then use thicken to create the spiral rectangle.

1. Sketch the outer radius on the face you want to attach it to.  I chose 4 in.


2. Create an offset plane (any distance as we are collapsing it later) and sketch on that plane the inner circle.  I chose 1 in.


3. On a perpendicular plane (may need to create one) sketch a line that pierces the outer radius and the inner radius.


4. Revolve this line around one of the two circles to create a cone surface.  (Choose surface revolve).


5. Apply a 2.5 turn helix to the surface.


6. Sketch on the face that you want to attach the spiral to.  Choose the 'Use' command and select the helix.  This will project it onto the face, which is the spiral we want.



7. Extrude the spiral as a surface the height that you want it to be.  I used the default 1 in.


8. Use the surface to thicken and create the surface on the face we want.  Make sure it is an "Add" to attach it.



Another approach I had was to sweep a rectangle along the helix and then use replace face on the top and bottom to flatten it.

jakeramsley

Is the spiral planar or is it 3 dimensional?  I can't tell based on the image.  If it is planar, you can create a helix on a cone and then project it with 'Use' command onto a sketch.  

stephen_sjodin

What you see in my image is a three dimensional rendering with the walls of the spiral twisting out from the centre hole.  I guess it can be hard to see when it's a static picture.  Here's another view that might work better.

.

Anyway, I see what you're saying Jake.  I'll give it a shot.  Thanks very much

jakeramsley

Looks like you have a 2.5 turn spiral that is flat.  What I would do is create a cone that has the inner radius at top and the outer radius at bottom and attach a 2.5 turn helix to it.  Then sketch on a plane and project the helix.  This remove the z-depth and flattens it into a 2.5 turn spiral.  From here I would probably extrude the spiral as a sheet, then use thicken to create the spiral rectangle.

1. Sketch the outer radius on the face you want to attach it to.  I chose 4 in.


2. Create an offset plane (any distance as we are collapsing it later) and sketch on that plane the inner circle.  I chose 1 in.


3. On a perpendicular plane (may need to create one) sketch a line that pierces the outer radius and the inner radius.


4. Revolve this line around one of the two circles to create a cone surface.  (Choose surface revolve).


5. Apply a 2.5 turn helix to the surface.


6. Sketch on the face that you want to attach the spiral to.  Choose the 'Use' command and select the helix.  This will project it onto the face, which is the spiral we want.



7. Extrude the spiral as a surface the height that you want it to be.  I used the default 1 in.


8. Use the surface to thicken and create the surface on the face we want.  Make sure it is an "Add" to attach it.



Another approach I had was to sweep a rectangle along the helix and then use replace face on the top and bottom to flatten it.

stephen_sjodin

Magnificent!  Thank you Jake.

I had one issue though.  When I thickened the surface, I did so towards the centre to keep the furthest reaches of the thickened spiral within the outer wall.  It didn't work with a thickness value of 1 mm - it didn't thicken at all.  It was fine with values of up to 0.75 mm.  I didn't see this behaviour when thickening away from the centre.  I realize that this is easily remedied by changing the dimensions of the base circle I'm starting with and thickening out rather than in but, as OnShape is in beta, I thought I'd mention it in case it's a bug.

Also, not all spirals are Archimedean like we've done here (http://en.wikipedia.org/wiki/Spiral#Two-dimensional_spirals).   I assume other spirals can be defined either mathematically with Python maybe (?)... or doing something similar to what was done here but applying the helix against an appropriately shaped surface based on a curved line.  I'm just putting this out there too.

Again, thanks.  

Cheers

andrew_troup

Ha! Reminds me of an interesting job I had to tackle recently in my old-school machine shop: truing up the three-start scroll from a (new) self-centering lathe chuck I'd rescued from the dumpster when a neighbour discarded it because it would not centre with sufficient accuracy. He'd had it on the shelf for too long for the supplier to entertain a replacement.

Turned out the reference bore of the scroll *was* dead true to the spiral, but a couple of burrs on the scroll tips had been missed in the deburring process at the factory (no, it was not from mainland China!)

It was an interesting challenge, working out the true centre from the spiral flanks using only an indicator and a rotary table.

stephen_sjodin

Andrew_Troup said:

Ha! Reminds me of an interesting job I had to tackle recently in my old-school machine shop: truing up the three-start scroll from a (new) self-centering lathe chuck I'd rescued from the dumpster when a neighbour discarded it because it would not centre with sufficient accuracy. He'd had it on the shelf for too long for the supplier to entertain a replacement.

Turned out the reference bore of the scroll *was* dead true to the spiral, but a couple of burrs on the scroll tips had been missed in the deburring process at the factory (no, it was not from mainland China!)

It was an interesting challenge, working out the true centre from the spiral flanks using only an indicator and a rotary table.

Cool.  So between the measurements you took and this software, you're all set to machine a replacement to sell to your neighbour  

andrew_troup

No, I had previously suggested I could rescue the entire chuck from the (shared) dumpster and have a go at fixing it for him, to which he replied he'd already bought a replacement chuck, and I was welcome to use it for one of my lathes if I could repair it and make a suitable backing plate.

I didn't have to machine a replacement for the scroll, just removed the (very hard to detect) burrs, and it was good to go!

stephen_sjodin

Andrew_Troup said:

No, I had previously suggested I could rescue the entire chuck from the (shared) dumpster and have a go at fixing it for him, to which he replied he'd already bought a replacement chuck, and I was welcome to use it for one of my lathes if I could repair it and make a suitable backing plate.

I didn't have to machine a replacement for the scroll, just removed the (very hard to detect) burrs, and it was good to go!

Yes, I figured that was what you would have done.  I was just kidding about building one for the neighbour.

jakeramsley

stephen_sjodin said:

I had one issue though.  When I thickened the surface, I did so towards the centre to keep the furthest reaches of the thickened spiral within the outer wall.  It didn't work with a thickness value of 1 mm - it didn't thicken at all.  It was fine with values of up to 0.75 mm.  I didn't see this behaviour when thickening away from the centre.  I realize that this is easily remedied by changing the dimensions of the base circle I'm starting with and thickening out rather than in but, as OnShape is in beta, I thought I'd mention it in case it's a bug.

I believe the issue is that the radius is so tight at the center of the spiral that trying to thicken in is causing the part to overlap on itself which is resulting in an error.  This is why it is acceptable to thicken outward.