Wrapping a sketch onto a surface

john_mcclary

@Jake_Rosenfeld
thanks for the heads up

dave_cowden

@MBartlett21 wow thats cool, thanks for the heads up!

MBartlett21

Jake_Rosenfeld said:

@MBartlett21
@john_mcclary

I apologize for the inconvenience, opRoll should have been released with an @internal tag.  Please feel free to play around, but the behavior may experience some changes over the next few releases, and there is a small chance that geometry created by this feature will change slightly from one release to the next.  Hold tight to use this in production work.

@Jake_Rosenfeld
Should this also go for the Hem feature (it does not have an @internal flag and it also uses opRoll).

hans_haenlein

This has become a long and interesting discussion thread, but my original request has not yet been addressed. I'm after a more general mapping function that maps any 2D curve or curves onto any 3D surface, not just a cylinder.
My understanding is that all surfaces, even those that topologically knit together to form a solid, are 4 sided parametric entities with whatever underlying math (most likely non-uniform rational b-spline or bezier). Note that sometimes one or two edges can collapses to a point, or a vanishingly small edge (like the poles of a sphere).
Two more important aspects (of surfaces) are the U and V parameters. These are values on the surface ranging from 0 to 1, used in the mathematical definition of the surface and for defining paths on the surface: for example, a trimmed boundary edge. Note that they are not proportionally spaced along the surface. A curve of constant U or constant V is known as an isoparametric curve, or U (V) line. In CAD systems, surfaces are often displayed with their poles of constant U or constant V values connected together by lines; these are known as control polygons. (straight from Wikipedia)
This means that every point on every surface can be defined by a single (u,v) parameter, where 0<=u<=1 and 0<=v<=1.
My request is that any 2 dimensional curve drawn in the same plane (the x,y plane for instance) as a bounding rectangular (or square)  can be mapped onto any surface, where one corner of the bounding rectangle or square maps to u=0, v=0, and its diagonal opposite corner maps to u=1, v=1.
What this mapping means in real life depends on how you set up the curve(s) on the flat plane, and how you set up the mapping surface. This is easy to imagine and set up for an extruded surface, gets a little more strange, but still useful, for a more complex surface. It doesn't have to be a 1:1 scale in either axis, but you can set it up to be that.

Jake_Rosenfeld

@hans_haenlein

This is the goal of the new opRoll interface.  After cylinders we will be building over time to support other developable surfaces.  We are also working on a built-in feature so that users do not need to implement a custom feature on top of opRoll.

@MBartlett21
Because of the planned change to opRoll, yes, a sheetMetalHem may go from failing to passing in an unexpected way. We've done some categorization of the opRoll change, though, and it is not likely to cause major problems.

lana

@hans_haenlein
Curve  modification you are describing is not quite the same as a result of opRoll. opRoll is designed to do length preserving roll onto developable surface from plane or from developable surface to plane (unroll). The functionality you are describing could be implemented as a custom feature script using evFaceTangentPlanes() to generate points on surface and opFitSpline to generate 3d Curve.

hans_haenlein

Thanks Lana - this sounds like it would do it. Now I just need to write the Feature Script...

chris_bottino

Jake_Rosenfeld said:

@hans_haenlein

This is the goal of the new opRoll interface.  After cylinders we will be building over time to support other developable surfaces.  We are also working on a built-in feature so that users do not need to implement a custom feature on top of opRoll.

@MBartlett21
Because of the planned change to opRoll, yes, a sheetMetalHem may go from failing to passing in an unexpected way. We've done some categorization of the opRoll change, though, and it is not likely to cause major problems.

Hi Jake - so is there an unstable "beta" way to use/test opRoll now to project a sketch onto a non circular surface?  Thanks

Jake_Rosenfeld

@chris_bottino I can't find it right now, but in another thread we mentioned that opRoll is now stable and fine to use; but we have not yet released a feature for its usage (though I bet that @konstantin_shiriazdanov and @MBartlett21 have been playing around with it).  Although the interface is now stable, it does only support cylinder wrapping.

curtis_heisey

@Jake_Rosenfeld  I would be interested in details about how to use the opRoll function and any examples of it's use. I'm trying to unwrap a cylinder onto a plane to use as a cut template.

https://cad.onshape.com/documents/73c28e94a3dec12ce27a24d2/w/32ab8a2dac5a3c91b153b8eb/e/9dd5bf2c4f13b013c37ce4fc

Jake_Rosenfeld

Hi @curtis_heisey !

Sorry for the delay, I was on vacation.  We actually renamed `opRoll` to `opWrap` after shipping it.  The best way to see an example of this is in the Wrap feature itself: https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/5e2ac00ef43da299ccb2ff00 or the opWrap documentation: https://cad.onshape.com/FsDoc/library.html#opWrap-Context-Id-map

A couple notes:

• opWrap will not be able to unwrap a solid cylinder, it can only unwrap faces.  If you want to unwrap a constant-thickness cylinder, consider designing it in sheet metal.
• opWrap cannot infer a "cut line" onto a complete cylinder face.  You'll have to split your cylinder face if you want to unwrap it, so that opWrap knows where the split is.

Let me know if this is not sufficient, and I can take a deeper dive.

samuel_byrne

I needed to engrave a pattern into a contoured surface (near cylindrical but not). I was able to achieve this effect with Boolean Plus Custom feature.

Steps:
1) Make cylindrical surface just bigger than needed surface.
2) Offset surface of desired face to engrave by 0
3) Thicken offset surface by desired depth of engrave
4) Create sketch to wrap 
5) Wrap sketch onto cylinder
6) Thicken wrapped surface though offset surface part
7) Boolean Plus to Intersect (creates part that is material to remove)
8) Boolean Plus to subtract engrave part from original part

steven_van_luchene848

Hi @Jake_Rosenfeld. 
been following this thread looking for a an answer to a  specific problem/challenge. 
I need to be able to "wrap" points/ positions to a cilinder mantle preferably have mate connectors at specific points on the cilinder mantle so I can later add features (nozzles,  basically cones) to those specific positions. The nozzle layout (pattern) is drawn out on a flat surface and projected onto the cilinder. so wrapping seems to be the logical command here, but apparently the wrap command does only take (closed) profiles. no points or mate connectors.

long story short. Is there a way to "wrap" mate connectors to a surface? 

a (very messy) example can be found here: 
nozzle_feature | Part Studio 1 (onshape.com)