Can't select helix curve with "Use" command

florent_herbinger

I'm following @jakeramsley tutorial for creating a spiral (https://forum.onshape.com/discussion/809/spirals); I'm interesting in creating a spiral sketch with a non-zero thickness, and this tutorial gets me most of the way there. However, I'm stuck on step 6, where the helix curve is selected with the "Use" command to project on the sketch below—I'm simply not able to select the helix.

I have outlined my steps here:

1. Make a circle sketch with a 45mm diameter on the Top plane (the sketch plane where I want my spiral sketch to be located)

2. Draw a horizontal construction line going from the center of circle of to its edge (used later for creating another sketch plane)

3. Create a 10mm offset plane from the Top plane (titled "Plane 1") and create a circle sketch with a 10mm diameter

4. Bring the 45mm circle in "Sketch 1" to "Sketch 2" with the "Use" command, and make the center points of the two circles coincident

5. Make the same horizontal construction line on the 10mm circle

6. Make a curve point plane (titled "Plane 2") by selecting the edge of the 10mm circle and the intersection point between the 45mm circle and its horizontal construction line

7. Sketch a line between the 10mm circle and the 45mm circle on "Plane 2"

8. Revolve the line around the 10mm circle as a surface

9. Create a 3-turn helix on the face of the revolved surface

10. Now here is where I am stuck. When I "Edit" Sketch 1 and click the "Use" command, I am not able to select anything outside of Sketch 1, including the helix.

Any help would be much appreciated!

tim_hess427

Modeling in onshape is "history" based - each feature in the list can only see the features that came before it. Since Sketch 1 is at the top, it can't reference any other features. If you want to reference your helix, you need to add your sketch below it. 

nicholas_radzykewycz

Another thing you can do is skip making a cone entirely, and use the featurescript version of opHelix, which has Spiral Pitch available directly so you can make your spiral without needing to use a reference geometry. I will add this to my list of featurescripts to make for a spiral creator that will give access to this functionality of OpHelix in the UI:

Here is some example code from my upcoming NPT thread maker that displays OpHelix being used with a table lookup for automatic resizing:

opHelix(context, id + "helix1", {
                "direction" : Normal.normal * meter,
                "axisStart" : CenterPoint,
                "startPoint" : StartPoint,
                "interval" : [0, table.length*table.TPI],
                "clockwise" : true,
                "helicalPitch" : table.pitch * inch,
                "spiralPitch" : table.Spiralpitch * inch
        });

nicholas_radzykewycz

@florent_herbinger I have created a simple featurescript that will let you use the spiral pitch system. It's not very polished code yet but this should get you what you need. Simply set Pitch to 0 to get a flat spiral. Spiral Pitch is defined as the horizontal distance between the same points on the helix for each rotation. Height here is supposed to define the height of the object but it gets sort of weird with flat spirals so I'm not 100% sure what it's doing when the Pitch goes to zero. It still works but you will have to play around with it a little to get precisely what you want.

https://cad.onshape.com/documents/a8088340dd05ad7ca39ec62a/w/e7ef6858314d4f2c4de13b98/e/1fa5a43942263ba31ea830ec

florent_herbinger

Thank you for the quick reply @tim_hess427 !

When I reordered Sketch 1 to the bottom, all the other features above broke since they depend on Sketch 1. It appears that I have a dependency loop. I therefore had to create a 45mm circle as a separate sketch to get this referenced spiral method to work.

Thanks a lot for the featurescript @nicholas_radzykewycz !

It will make it much easier to create 2D spirals on the fly. I will try it right away !

florent_herbinger

Ignore this redacted post; the very slow approval process of OnShape forum posts resulted in this message, posted before my message above, being no longer relevant.