I built this solid in Rhino. I need to do the same in SOLIDWORKS with real dimensions. Please guide me by including your file. Note that all the circles are in the same radius and they have just been projected nicely all over the object.
Dennis Bacon wrote: Oh yea,, I remember seeing that before. The ole sphere in the hole trick. Or should I say sphere to make hole.
Dennis Bacon wrote:
Oh yea,, I remember seeing that before. The ole sphere in the hole trick. Or should I say sphere to make hole.
Basically, I used Face curves to get the surface data....then placed a point at each intersection of the curves (although I see that using the segment tool might have been a better use of my time [Edit: unless you are using anything below SW 2017]).
(from what's new SW 2017):
Then I created a single sphere at the one point and then used a sketch driven pattern to pattern the spheres.
Then I created a split line on the facing surface at its intersection with each sphere.
Then I offset the surface that was outside the circles created by the split lines 0in.
Then I deleted the original body and the spheres, which left only the offset surface with holes in it.
Then I thickened the new surface.
(edited for clarity)
Use sheet metal for it
1)Create a flat flangle
2)Add holes (use pattern)
3) Draw a sketch and use sheet metal sketch bent feauture
(I just guessed at dimensions)
Is it the end of the semester with several projects coming due?
What if the base solid be a free-form complex shape?? (Not an industrial simple one)
See Dan's model - you can create any shape you want
Make any shape you want with the base flange command in the sheet metal commands.
Unfortunately most of us here have jobs that pay us to do this work and it takes us time to do your project for you. We are willing to help with advice and suggestions but we can't be doing all your work for you. Besides it is slightly unethical for us to do your school work for you unless you want to place our name on your diploma along with yours. Wayne has created a good starting model for you to work off of and Dan has created a model where you can follow the feature tree on how he created the model.
Or you can use flex feature - see this sample
Alex Write wrote: thanks,What if the base solid be a free-form complex shape?? (Not an industrial simple one)
Alex Write wrote:
You mean like this?
I'm going on record to say "It's not possible in SW". Unless someone cant prove me otherwise.. It would be nice to have your file, maybe converted to step, for us to take a look at. A sheet metal loft (freeform) might be a possibility but it's hard to say without seeing what your surface looks like.
For example, I want to provide the same feature over this free-form solid (holes all over the object).
Please not that the simple curve projection results in wrong holes especially in highly curved areas.
Please look at my next reply. I provided a STEP file showing what I meant and what I'm going to gain.
Possibly something like this. Takes a bit of work. Face curves and hole wizard holes at intersections.
Probably a better way of doing this would be to use the sketch segment tool in order to get evenly distributed points.
You could do that on each horizontal line???
Here is a start but you will have to modify it.
Alex Write wrote: For example, I want to provide the same feature over this free-form solid (holes all over the object).Please not that the simple curve projection results in wrong holes especially in highly curved areas.
Alex Write wrote:
Can't get segment to work. Maybe because it is a spline?
Yes, I recall that You can do a sketch driven pattern with the sphere. I had tried to do that with the hole wizard hole but that didn't work so good. I'm quite certain that your approach is the best and although it may seem complicated, it really isn't. Alex Write,, IMHO, this is the way to go.
use the sketch points (Edit:.. option).. It works on my spline.
I couldn't get hole wizard to work on the OP's part either, because the some of the areas of the surface are concave and convex, which means that the hole fails in the convex areas. Although, maybe it is in the way I am doing it, or that I am SW 2015.
Dennis Bacon wrote: use the sketch points (Edit:.. option).. It works on my spline.
Yeah, I tried both options and it won't work. I am SW 2015, so maybe that is it?
Yes, if I remember correctly that was a 2017 enhancement. I did mine on 2018
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