Unfolding cylinders (wrap)

akendall1966

Hello,

I don't currently have sheet metal add on to explore. But can sheet metal unfold a cylinder to flat, and re-fold back to a cylinder after cutting some features into the flat form?

Cheers
Adrian

Jim Canale

I created a rolled cylinder then unfolded it with the K-Factor the program selects as a default. The unfold went smoothly. The unfold created some nonsensical bend lines and angle measurements on the unfolded blank. Whether the blank size was calculated correctly is up for debate. I'm not certain I know how to calculate the length of the neutral path a cylinder.

akendall1966

Thanks Jim,

That's useful to know.

Found this, https://www.cmrp.com/blog/plate-rolling/calculating-the-developed-length-of-a-rolled-cylinder.html suggests for a large radius rolled cylinder K=0.5. Following the logic of the piece I would assume neutral path length would be the circumference of mean radius of OD & ID.

Thanks Again
Adrian

Jim Canale

I created a thicker cylinder (.2"), and unfolded it with a K-Factor of 0.5 That SHOULD produce a part with the neutral line passing exactly through the center of the part. I then compared the arc length of this neutral line, with the blank length calculated by the program. They were NOT the same. I don't know if this has something to do with the fact that the cylinder was a "lofted" bend consisting of multiple segments. I will increase number of segments and try again.

Jim Canale

Yep! That's what it was. I increased the number of segments in the lofted bend to 100, and unfolded. The length of the blank then approached very closely the arc length of the arbitrary neutral line.

Richard Webb

It does work to re-roll after cutting a familiar shape on the flattened piece. Tedious enough at ten segments, can't imagine rolling 100 ... although @Roy Klein Gebbinck probably already has a Lisp routine in mind to automate rolling it back up along the fold lines. ;-)

Would be handy in some circumstances if _ProjectGeometry could be extended from a planar projection to use a cylindrical or spherical projection.

akendall1966

@Richard Webb said:
Would be handy in some circumstances if _ProjectGeometry could be extended from a planar projection to use a cylindrical or spherical projection.

Yes - the ability to project / wrap a 2d sketch onto a cylinder in SW & Inventor then extrude / cut is leaving me a little envious on my current task. So even if tedious using sheet metal to do the reverse would help some.

Egor Ermolin

Hello Adrian,

In order to unfold cylinder in BricsCAD one indeed has to increase number of samples to some high value, near 100, as Jim did. kFactor for lofted surface is 0.5 However, there will not be way to refold it. We will consider with team improvements for cylindrical surface unfolding.

Alternative way to try is to create single flange for hole, SMBEND it and then subtract from cylinder. Not the best way, since positioning will be complex, plus SMBEND will assume that flanges have to be created.

Best regards,
Egor

akendall1966

Hi Egor,

Thanks for your reply. In terms of new features its actually being able to project 2d geometry onto a cylindrical surface and have it wrap around the surface like a sticker but then be able to extrude and cut the projected features. Using sheet metal to un-wrap a cylinder work on the flat from then roll it back up is a workaround I see on line in Fusion 360 to the issue of not having project 2d with a wrapping mode. I was curious if a similar workaround in Brics might work.

Putting this feature on the road map if not already in progress would interest me.

My application if it helps is I needed to cut helical slots into a cylinder surface to a depth, then have a a series of holes through the full cylinder wall in the bottom of the slots. I seemed unable to select the curved slot bottom to sketch of DM the holes. So ended up make a huge radial array of solid cylinders where the angle in between and height between levels allowed some of the array to follow the slot. I deleted all that where not need and subtracted those in the right place to for the holes. It worked but was hours and hours of work doing it this way.

If there a better way to model it I am happy to learn.

Regards
Adrian

Egor Ermolin

Hello Adrian,

The complete scenario will be reachable in some long-term period (after V19 release), since right now we are not focused on smooth unfolding of cylinder, needed to step back from 2D to 3D, but still approximate with lofted bend

However, it will be interesting to see some example you want to obtain to see if SMBEND solution will work

Please also note that you always can open Support Request, as well as evalute Sheet Metal for trial period.

Best regards,
Egor

akendall1966

Hi Egor,

Here's an example of what I am working on to share with the team.

Adrian

Egor Ermolin

Hello Adrian,

I would say that attached example is out of what we consider sheet metal:

• it contains holes on thickness faces (the ones which have thickness 30)
• holes are not symmetrical depending on the side of the part
  Thus if we call feature recognition and then unfolding, it will be slow (due to model size) and some of the features will be lost. Plus unfolding will not be regular, see attachment

I've tried some proof-of-concept scenario (see fold_cylinder.dwg from left to right):

• create unrolled piece of which we will roll to quarter of cylinder. I want to have internal radius equal to 200. Thus unfolded length is (2Pi)(R+kT) = (2Pi)(200 + 0.52) = (2*Pi)**201 = 1262.920246506 for R = 200
• Call SMConvert to recognize as flange
• Make a pattern element - let its X and Y dimension will be 1262.920246506/20
• Array it, then explode, the subtract from part
• SMFLANGEBEND by angle -179.9999999 R 200
• SMDISSOLVE to remove the features

However the result is not perfect at the connection of 0 and 360 degrees, next there is hole mismatch. Currently I can't tell if there is some mistake in my considerations or it is failure of the bending by such angle, you can try Sheet Metal trial and play with the approach.

So the conclusion is that Sheet Metal right now doesn't support complete cycle of work with closed cylinders with non-orthogonal holes, but there is some approximation to start from scratch. I don't think that we will improve closed cylinders in Sheet Metal in nearest future. May be, if there is user request (meaning argumented Support Request), we will expose part bending out of Sheet Metal, which will allow to bend parts and Pro license as Direct Modeling command.

Best regards,
Egor

Roy Klein Gebbinck

I have not yet looked at the dwg provided by @akendall1966. But creating a helical slot in a cylinder should be possible.

My approach:

1. _Sweep a rectangle along a helical path.
2. Create two cylinders for the rounded ends.
3. Either _Subtract the cylinders and the swept solid from a pipe solid for a through-and-through slot.
4. Or _Union the cylinders and the swept solid and _Intersect the resulting solid with a pipe solid to create a solid that can then be subtracted from a base cylinder to achieve a recessed slot.

akendall1966

Hi Roy,

Yes that exactly the approach I took but if you have chance to look at the DWG, there multiple interleaved helical slots, and every slots has holes in the bottom of it. Its all perfectly do able but vey time consuming and Brics got very slow to regen.

To be clear sheet metal approach is copying a workaround I have seen being used in Fusion 360, So would consider licensing SM it if the work around worked for Brics. But, sounds like its a no go. Wrapping 2D geometry around the cylinder surface and then being able to extrude or cut it seem the better approach and apparently is a feature in Solidworks and Inventor. Other wise its build up from 3D elements and sub / uni to get the final solid.

Thanks Everyone for taking an interest.

Adrian

Roy Klein Gebbinck

@akendall1966:
If I look at your slots I find that they are made up of 7 spline faces. If I subtract the solid from step #4 in my approach from a cylinder, the result is a slot with 5 faces, only two of which are spline faces. So I do not think that your approach is exactly the same. Having fewer (spline) faces may result in a more manageable object.

The task should not take a lot of time. You only need to create two temporary solids similar to my step #4. Add x cylinders for the holes to each, _Union both assemblies, create multiple copies (using _Copy, _Rotate, _Array etc.) and finally _Subtract all temporary solids from your pipe solid.

Roy Klein Gebbinck

I have created a similar model. Mine has 120 slots with 7 holes each. Yours has 60 slots with 10 holes each (slots at the top and bottom of your model are actually shorter and have fewer holes). On my computer my model opens 3 times faster.

akendall1966

Much appreciated Roy,
Traveling for few days now but will study when I am back in my office on Thursday.
Adrian