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sketching on a curved surface

S

sleep_flower

New member
hello all,


I'm modelling a concept for a new coffee mug, and i am having difficulty sketching on a curved surface. The surface is cyclindrical like a normal mug, and i want to add detail to it, but i cant select the cylindrical surface to sketch on. How do i go about it? View attachment 3303





here is thesketch for better clarification. as you can see there are two diferent materials. the white part was modelled using a simple revolve, but i want to add the grey material. the sketch shows it to be raised by a few mm's, but this has changed. Basicallyits not raised now, but where the grey and white materials meet there will be asplit line. It's this split line where i havent got a clue on how to do it...any ideas? you will have helped me so much. i got told i could easily do it on rhino, but i'm not a fan of that programme
smiley1.gif
oh and i'm using pro engineer wildfire 2.0
 
sleep_flower,

You might try to draw the shape, on a flat plane, as a datum curve sketch. Then project that onto the revolved surface. You can then copy the surface selecting only the area one one side of the projected curve, and offest inward to make the new area. Will you be making the grey material as an overmold step in the final product? There is also a "wrap" function if that is more suitable.

cheers...

M
 
Try creating a "cosmetic groove". Select the cylinder surface as the reference, then create the sketch on a plane that is offset away from the surface, then select or flip the projection direction toward the surface. Now create your sketch. Whatever you sketch gets projected onto the reference surfaces.
 
hey magneplanar, thank you for your reply. The grey material was going to be an overmould by 2mm over the white ceramic, but now its going to be merely flush with the white ceramic, but seperated with a split line so it looks like there are still two materials. your idea of drawing the shape ona flat plane, but how do i set up the datum curve sketch. apologies i'm very amateurish when it comes to doing organic shapes in pro-e and messing around with datums


thank youu
 
sleep_flower,

imagine what the shape would look like from one side view looking towards the mug, as appinmi said, you can place the plane outside the shape you already have. then you can wrap or project the shape onto those surfaces. there are options for projecting normal to the surface or normal to the plane you made the sketch on, try both to see the difference.

no apologies needed, we were all there at some point...

cheers

M
 
ahh thank you, the only really successful feature was sketching what it would look like from the side on an offset plane then projecting it onto the surface. BUT after that even though i made sure that when i sketched the lines it was closed, it projects onto the surface open as shown below, so i cant extrude it. grr so annoying, is their something simple i'm missing. half way there!! View attachment 3304
 
oh please note the picture above is me just messing around, hence why it looks nothing like my sketch. haha i'll post my final model up when i've done it properly as soon as i've found out how to do it
smiley1.gif
 
sleep_flower,

you have the idea...now you can handle this a few ways. you can offest a line from your original line and make a surface between the lines, or you might copy the whole surface and select just the details on one side of the curve. not sure if you need a closing curve, but you can project a line at the top, across the two open lines to close out the circumference.

how thick is the groove you want between white and grey? .5mm?
 
note: copy the surface and build with the copy...not sure what you are extruding, if you mean thicken, I prefer not to use that or the shell function...call me crazy hahah
 
hey magneplanar i've managed to close the two open lines at the top. now how do i make the groove and yes good guess i'll have a mess around with .5mm, should be a nice split line!now i thought i could of done it with the extrude function...the thicken sketch one option, but when i select my sketch that has just been projected to extrude, it is having none of it. grrrrrr
 
for myself I would build a surface in the shape of the groove..full width ( 0.5mm or whatever) I would then offset that surface and cut out the unwanted material with a closed quilt...if you want to thicken, you need to thicken a surface and not a line so complete the surface.

you could also use the line you made on the main body, in the image above, and sweep a cut to remove the material you do not want.
 
right i'm back to square one again...as you can see i have projected a sketch onto a curved surface...all i want is to where that sketch is be a 0.5mm groove in the surface...i'm lost. please help guys....magneplanar i'm so confused from your last comment with creating surfaces and using a closed quilt. sorry to keep asking, its just totally annoying meView attachment 3305
 
sleep_flower,

the surfacing method may be more than you need. you have a curve on the surface, use it for a simple sweep cut to remove the material you want.

like this:
View attachment 3306
there is a way to use a surface for this but it is more complicated. I try to avoid this kind of sweep if possible since it has a tendancy to roll like its falling off the rail(trajectory). In your case it should be satisfactory. If I have time I will do my other method and take a picture.

cheers..

M
 
alternate method:

if I make this into a surface quilt then I have many more options.

View attachment 3307

I can remove the area of the groove, remove the whole area where an overmold would be, or make complementing parts if they are an assembly by changing what directions I merge the surfaces.
such as:
View attachment 3308



Edited by: magneplanar
 
why dont you try with offset feature, u can select with draft option from the dashboard and make a sketch and it will be done by onlyone feature.
 
Zaki,

Just tried it...with the right sketch I was able to get an offset, but I was not happy with the direction control. The resulting surface would still need more attention before being suitable for material removal, correct? solidify did not work yet...

I am not sure what the sketch should look like to get the surface as shown above. I tried a simple circle at the bottom and the surface worked, but I think that is probably not the right shape. I also tried using the curve that is projected on the main body.

I would think that no draft is needed since the groove would all be undercut, and if you remove material for an overmold it would not have undercut features. Draft with offset is a handy tool to have, but not sure how to work it in this situation...care to make a screen shot? hehe

M
 
Magneplanar, thank you ever so much, the sweep cut worked a treat, and its a function i've never used before along with projection so i really appreciate it....heresjust a quick rendered image of it done on flamingo showing you the shape of the grip.


View attachment 3312


Again thanks again and i'll keep posting up progress shots of it, and of course a final image. just the handle to do now..nightmare!!


craig
 
sleep_flower,

glad to be of some help...as soon as you find a new function someone comes along with an even faster way, but it is a learning process. keep exploring what is possible and looking into new features...

cheers,

M
 
hello all again...i'm doing the handle at the moment, and i was just wondering. can you extrude at an angle on say a 90 degree plane, or do you have to set up a plane in the direction your going to extrude becasue you can only extrude at 90 degrees. if thats the case i think i've found a problem that i cant get around. so frustrating :)
 
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