Hello all
I am trying to fill the space between two bodies (corrugated plates). I wanna use this filled space as new body. What do you suggest?
I tried to draw a box around two plates to use combine (subtract), but when I select plates to be subtracted from the box it gives an error prompting to select another feature.
Thanks in advance.
Hello,
i would recommend to add some planar surfaces (to get an inner volume) and then to use the "Intersect" feature.
This should work for you..
Cheers, Heiko
If I got you point right, I have to add lots of plans. In fact for this kind of solution, I can draw sketch at the end surface of each plate, then try to extrude bodies to fill the gap. I am curious for a more advanced technique, using commands and abilities of the solidworks
I don't know if it takes "a lot" surfaces - hard to say with just on screenshot.
But i've said nothing about "extrude bodies".
Have you had a look at the "intersect" feature - i think the answer is "no"...
Agreed....intersect is the way to go here. Would be very simple and easy (depending on the complexity of the edge of the part). But if you have 4 flat sides.....you wouldn't even need Planar surfaces.....simple reference planes would work.
If everything is square and parallel then it could be as simple as using a face for the extrude plane, use the Convert Entities sketch tool, and Extrude "Up to Surface". No cuts needed.
Hi Glenn,
if I well understood, looking at the picture that Ram shared, the corrugations are perpendicular each other.
So may be you need to apply your solution twice starting from a middle plane, first upwards and then downwards.
thanks for your comment. The direction of two plates are different. So yes as I said above I can extrude two (or more) sketches in two directions to fill the space. since the geometry has many edges, and I have to draw a couple, and some cuts will be needed, so maybe another "cleaner" method can be suggested
Can you create a new part in the assembly, convert entities to 'grab' the existing edges of your two parts and loft surfaces between them?
loft on this geometry does not work, the conduits are not in front of eachother and they cross eachother.
the solution is something like to combine them then omit the bodies that are not in interest, but I dont know why I cannot cut the plates from the surrounding box.
You can draw 3D lines between vertices of the converted entities and create surfaces between the lines. It may not look pretty to start but then you could put the whole thing in a "box" and grow the sides to fill to a face in a single direction.
Another way would be to throw a plane exactly between the two and sketch (I'm assuming) a square then 'extrude to next surface'.
that is what I was thinking!!! really any plane between the two and extrude both ways up to surface should work.
James Riddell wrote:
Another way would be to throw a plane exactly between the two and sketch (I'm assuming) a square then 'extrude to next surface'.
A nice simple answer. I like simple. I am simple.
Another option could be to start drawing the filling first. You can start from a thick plate and cut using the sketches you've done for the corrugated plates. Then add a thickness body on both surfaces. Could it be faster?
yes I think you are right, I can draw the middle one first then cut the pattern. finally extrude the pattern from sketches. It is much faster, thanks
This is what I would do..
Create a "New" Assembly and add the parts you show above and save the assembly. Then add a "New" part Insert/New Component save it, then edit the "New" part and add a rectangle sketch just to the outside of the parts and extrude up to surface in each direction, if that doesn't work then I would extrude a certain thickness dimension and then use the cavity tool to trim out the other two parts, then trim with Cut Extrude as needed. Should be pretty quick..
Can you upload your part?
Thank you, yes this is another solution to go to assembly and use Cavity tool. I will try it now.
Another solution could be to create the filling first, then "copy body" and use "Shell" on the new body selecting 4 side faces as open faces, and adding thickness outside.
My solution would have been:
- sketch an rectangle, fittet to the sides (edges) on Top Plane.
- extrude a surface
- use Intersect
Done in 30 sec...
Another way would be to throw a plane exactly between the two and sketch (I'm assuming) a square then 'extrude to next surface'.