Hi all.
For some reason, I'm always having this issue with lofted/boss feature. I'm sure it's due to my lack of understanding of how it works. I'm just trying to create a lofted bubble object per the image below. It keeps giving me this "at least two profiles are required to make an open loft). I'm not sure whether I understand what it means since I thought I have all of the lines already interconnected. Please advise? Major headscratcher for me among many other things.
P.S.: Admin, my apology for posting the question on the wrong page again. Should have click ask a question instead of "ask it" in the forum. Have no way of moving it to question page after page is created. My bad.
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SolidworksParts And Features
Thanks Paul.
I hear you. The only problem I have right now is seeing where I did what you suggested. Price of learning, ey? /ScratchingMyHead..
Separate plane for each guide curve will definitely work. But some times more than one guide curves on the same the plane also works. Do you know the reason?
I know you've already figures it out, but just so you understand why it wasn't working initially, look at the PropertyManager in your original screenshot. You have all selections in the profile selection list and none in the guide curves. You also have a plane selected in the profile selection list which is not an appropriate profile.
-Jim
Hi Dude,
Is there a particural reason you want to make it using loft???? I tried but no matter what I wasn't able to select all four splines separetly (like surface magician shows - I always select the whole spline thus the loft could not be done) but as SWX allows us to make things by many more ways - I used revolve (you don't even need sketch3 for that) and it worked fine for me..
EDIT: just found how to select splines separetly (shame on me for not finding out such an easy thing faster:) ....but the final shape isn't perfectly round!!??
or am I missing something in feature manager menu which makes it round??
(and before somebody asks, yes I did the sketches of splines the same size..)
I used the existing profiles in your model to build the shape without adding any extra sketch which you can control the curve to have diff. shapes
Dang, that's a wicked graphics. Fun once we all figure it out, right? Not fun when I was banging my head to the wall wondering what I didn't do right... LOL. Thanks again, man. Very educational... Now I just have to figure out how to do the "shell" since the round stuff in front supposedly a whole and the graphic should be an empty shell like an eggshell with wall thickness. That'll be a different posting, I guess...
..I knew you'd figure it out!... in this case, you need to choose the "group" option.
..you reminded me of how much fun a closed loft like yours can be! (image and file attached)
Thanks for showing me how it works with the open group. Not sure why it didn't give me the option on how to select the open group. I caught it by accident. What I did was, I click Lofted surface and on the "Profiles" box, right click and click on "Selection Manager". Then, left click on the line>right click on the line and it selected that line as "open group". Keep clicking on the rest of the lines and I remember to click on "close lofts" on the options on the bottom left. That just does it. Also, you use "Lofted Surface" instead of "Lofted Boss/base".
Thanks for showing me how it was done, Paul. Thanks, everyone...
Christian, yours look different using the boundary surface which I think it looks interesting. Thank you..
I did not add a circle, it lofts as is.
Hmmm.. Thanks, everyone. What did I miss? I tried it all and it keeps on giving me the error on the image I originally attached. The only thing that's different is I saw you guys added a circle or two in the middle with pierced point. Is that what I missed? Thanks again, everyone.
..hmm,.. seems to work fine? (image)
Ok! I got it
Did you add a circle in the middle
This is 2018v. You can open it. This is look like an egg shape therefore I added a profile in between.
Maha,
Interesting model. Can you repost without realview graphic so I can see it better
Hi Marek.
I think the feature manager is what enables me to select each of the splines as a group. I tried it without the feature manager and the error you see in my original posting graphic. As to why I choose to use the Loft? No reason actually. Cuz that's the one that works for me for this experiment and it actually generated pretty round but not perfectly round. If I needed it to be perfectly round, I'll do what Maha suggested. Your "Revolve" approach works as well. This is why I love SWX. There are so many ways to achieve the same goal. However, in my case, it won't work because the height for the top curve and the bottom curve are different. Unless revolve can use 2 curves as the guide line.
Hi Jim.
Good catch with the plane (I didn't even see it) and thanks for the side note. So you are saying that if I choose 3 of the splines and use the last spline as the guide curve that'll work? I tried what I think you had suggested and I can't even select the sketches in the profile box now. Strange how I got it in the original post graphic.
Hey Le Dude,... glad you see the fun in it.. you need to play to get use to it (I attached the file above).. and it does help understand the limitations.
The shell should work?... but, run "Check Entity" and select Minimum Radius of Curvature to help you know the thickness limit of not?
Hello Le Dude,.. using a vertical construction line is a old habit from the past way and how I prefer to constrain,... alternately, you could not do a line and easily make the splines perpendicular to the centerline (image)
Thanks, Paul.
Very interesting approach. I think I see what you did there... Interesting that you can create a tangent at the end point for the vertical spline and middle construction line and yet it didn't change the shape. I tried to do the same and it bent around like crazy. I'm speculating the additional construction circle pierced to the vertical spline lock the spline from going crazy. Did I get it right? Thank you again. /ScratchingMyHead.
..file attached above.
For the life of me, I can never get the damn tangent working with me. Not just for this part, but also many other places... I tried to tangent the splines and everything light up like a Xmas tree. What did I miss? Mind sharing with me what you did with your file, please?
..make sure your splines are tangent at the end and it should thicken/shell (image / file attached)
Well, I tangent the relationship at the tail tip and also at the front round hole but I can't close it because it said I can't knit the sheets together. I can see there's a missing line on the front round hole to connect the last one. What did I miss? This time I'm using the Lofted Boss/base instead of "Surface Loft" Hmmm.... Please advise?
Always perfect time to drink from any time zone. Thanks, Jim. No worries at all, Enjoy your vacay in Ireland... Thanks for helping out...
Thanks, Newell for the advice. Perhaps I'm just not understanding what you are trying to tell me. Do you mind showing me in a picture what do you mean or save the file with your suggestion? Sorry, I'm one of those people who learn by visual. Thank you again..
Yeah, the minimum curvature per the checking entity is 1mm and the thickness that I select is 2mm. The other issue that I see is when I look at the picture, the inside loft empty shell looks like an egg but it doesn't have an even skin thickness. I wonder whether I need a different strategy to create the loft so that the skin will be even at 2mm and not looking the way it is right now.
Perfect time in Ireland for a drink as it's lunch time now in California
Well, since I'm retired and don't work anyway, helping out on the forum during vacation is no different than any other day!
BTW, this is being sent from a Whiskey and craft beer bar in Ireland!
-Jim
Jim,
You'd better enjoy your vacation !!
https://www.themuse.com/advice/how-to-keep-work-from-ruining-your-vacation
I'm actually on vacation with no access to a computer so can't actually check out your model to see how you've structured the sketches. I was simply going by your screenshot to point out there are multiple problems with what is shown in your selections lists that would make it fail no matter how your data is structured. Please go by the advice of the others in the thread for more specifics since they can access your actual data.
-Jim
All the more reason to define your sketches.
Your profile sketches are not tangent to one another at the tip.
original sketch thickened:
Corrected sketch thickened:
Follow the steps in Pauls image. Use RMB to get to the selection manager and group select your outer splines for the profiles and use the hole sketch as your guide. You can also try lofting from the hole sketch to a point. Or RMB on your loft feature after the fact and elect to add an additional loft section for further control.
Regardless, I would suggest fully defining your sketches at the very least.
I wonder whether the follow-up question should be created in a separate post? I put it here just because I think it's related to this one design. Once I have figured out how to create the eggshell, per your suggestion, when I tried to thicken the wall, I can't thicken it because of this error "failed to offset or face could not be deleted". Not sure what that means, I tried all of the thickness directions and it all gives me the same error. Any thought? Or perhaps other approach?
Is this what you want