Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

2d profile of a surface with curvature

S

smilingdragon

New member
This is the profile of a sticker on a solid(whose surface looks similar to that of a computer mouse body). it has a curvature. i need to make the 2d drawing of the sticker for manufacturing it. please let me know if we have any option to bend it to get its 2d profile.
i have tried flatten quilt, but it does not work as this curvature has tangency at more than one point.
 
can you convert it to sheetmetal? andthen flatten it ?


but yes...can upload the file?


//Tobias
 
thanks for upload but i can't open it on WF2
smiley19.gif
 
Yes, tried converting the surface to sheetmetal with 1mm thickness. But the flatten option was not highlighted, i din know how to proceed further.
 
I have tried the sheet metal tools in SolidWorks and they complain from the double-curved nature as well.

I have a trial version of Rhino here, now, I am not claiming to know the application because I have very rarely used it so maybe this isn't accurate. But I was able to flatten the surface. The Rhino command for it said accuracy will be lost either way, so take from it what you can get.

The material will matter as well and of course that wasn't taken into any account here.

I'm just trying to help
smiley1.gif


2009-06-03_090252_2d-profile_rhino.zip
Edited by: Kevin De Smet
 
You aren't going to be able to flatten that surface. It's not a Pro|E problem, it's a geometry problem.

The surface is curved in two directions. In order to have a surface that will flatten without rips or distortion (compression), you need what's called a single ruled surface. A single ruled surface is curved in one direction, but sections cut normal to that will all be straight lines.

A cylinder or a cone are good examples. Cut a cylinder normal to the axis and the section is a circle. Cut it through the axis and the section is a straight line. A sphere is not, no matter how you slice it, you get curved sections. That's why maps of the globe are either stretched at the poles or split into 'wedges'.

There are no straight line section on your surface, so it's not 'developable' (it won't flatten.) You'll have trouble with this in production as the decal won't sit properly. It'll wrinkle and won't stay down. You need to redesign your part to have a developable surface for the label.
 
Interesting that Rhino will flatten it. The 'accuracy lost' statement means that in order to flatten it, they either stretched or compressed the surface. Do a comparison of surface area before and after to see which. Of course, it's possible that some parts were compressed while others were stretched.

I suppose that with the proper label material, you may be able to stretch a label onto that surface, but I bet it's going to be a trial and error process to get it right.

We can talk about it all day long, nothing like a mock up to see what's really going on. Make an SLA or CNC of your shape and try to cover it with tape and see if it works.
 
I have to agree on this one, I don't believe a material-less flatten will help you much - like the one I achieved in Rhino. Let alone the theory behind it and why Pro/E won't touch it with a twenty-foot pole.

Keep us posted!


Edited by: Kevin De Smet
 
thanks for the replies friends. your assistance is much appreciated. we wil take the profile from the rhino model you have provided and wil use the trial and error process to select the exact shape. Wil update the outcome.
 
Hi Kiran


please try to copy its boundry curve then project it onto a solid planner face or on a datum plane.
 
yes, we got the boundary curve by projecting the surface
to a plane. But the cross section does not give the
actual area of the surface(sticker) it is less than the
actual surface.
 
another technique I can suggest that make a two curves on that surface, one horizontal and another vertical (must end at boundry). Then go to measure, pick curve length, pick feature option then measure these curves, now make another part, and make a flat surface in it. use length and height according to measured curves and trace this boundry on it. May it will solve your problem. If you can wait untill sunday, please email me the part, I will do it for you.
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top