Hi, can someone please help me design a part that looks like the one in the attached picture.
The best way I can describe it is if you take a cylinder and remove the front face and replace with this repeating pattern of alternating rungs. Then you also remove the back, top, and bottom of the cylinder. Lastly, there is a spine on the right and left side holding the ends of each rung. All the rungs and spaces between them are equal length.
Thank you very much!
Do you have any clue on sizes
Hi John,
The height should be four centimeters, so the whole thing is quite small. The rungs should account for 75 percent of the horizontal distance between the two spines (so only 25% of space between the end of a rung and the adjacent spine). Only 3-4 mm of vertical distance between the rungs. Lastly the width of the whole thing should be about 2.5cm.
Thank you very much!
Is this a top view? -
Could you sketch the other two views?
Have you made an initial attempt at this "part"?
Can you attach your file here?
Hi John,
This is the front view.
I have redrawn it and included a top view as well. I added little bridges between the rungs.
Thanks again for your help, I sincerely appreciate it.
Best,
Mike
This could be done in simple two steps.
Here is a quick picture, shape/dimensions not exact.
Hi Deepak,
Thank you for sharing this. Can you please provide a bit more details? I am confused about how you got it to curve with only these two steps? Also, what did you sketch?
Thank you very much.
Best,
Mike
Mike,
I extruded an arc. And then created a sketch for the cut extrude. The sketch is different from what you need but that can be managed.
I would doubt if this is correct as cut on the curve is going straight instead of normal/perpendicular to the surface. So if you need the cut normal/perpendicular to the surface, model this in Sheet metal (again same two features)
Thank you for sharing this. Can you please provide a bit more details?
I am confused about how you got it to curve with only these two steps?
See my response above. Let me know if more details are required.
Or you can create a curved base flange (in sheet metal), flatten it add a cut on on it and the bend it again. (Advantage being you can dimensions the cut on linear scale).
Hi Deepak,
I used the Sheet Metal approach and have a question. Below is my sketch ( I unfolded a semi-circular cylinder)
Instead of sketching the area I want to remove, I sketched the area I would like to keep. How do I extrude cut out everything around my rectangular sketches?
Thank you for your help!
Make sure you've used the unfold option in the sheet metal to flatten the semi circle before doing cut extrude.
And when you do cut extrude, simply select flip side to cut (if you've only one contour). But your picture is suggesting that there are multiple contours, so while doing the cut, select the area you want to remove under contour selection.
According to your sketch Mike there is only one part shown above - Basically if you split what you show above and keep the right side, that same part will work on the left side...
In the cut-extrude feature, use the 'Selected Contours' option to select the region you want to cut.
Thank you very much, design worked and 3D print came out nicely. I would like to add small tunnels to each rung and have run into a small problem. I created the tunnels (pic 1) but when I fold it back up they disappear (pic 2).
What am I doing wrong?
Thank you for your help!
Best,
Mike
I know you asked Deepak - pretty late from where he lives - so here is what I would do -
Select the one of the faces and draw your circles (red) -
Do a cut revolve by going to view/temporary axis and select the blue line as your revolve centerline
Thanks John, will do this. Why doesn't it work the way I did it? Just curious.
Is the design basis Sheet Metal ??
If it is that would be one reason, apparently it needs to be a solid model less any voids etc....
Yes it is Sheet Metal
Did you added them after flatten feature? Either way, you can't have like this. So go with John's method.
What I think youre trying to achieve:
YOu can creat the curved surce in sheet metal
.unfold>cut your patter>fold again
This way you can get the falt pattern for machining
Late to the party here...but I have an idea...two revolves and a few boss extrudes. I didn't take the time to add the connecting boss extrudes between each finger, if I had there would only be one solid body.
The profiles for the revolve contain the circle, to create a tube in each finger. ( You could fillet the rectangles right away to create a nicer looking finger, when you do the revolve.)
The Boss-Extrudes use the convert entities tool to get the curve of the fingers. Just add a line and trim.
See attached part file.
How thick is your sheet metal? How big are the holes you need? How do you plan to get holes in the sheet metal in that direction?
I dont htin k he intends to make it out of sheetmetal . but to use the sheet metal functions of solidowrks would be avdantageous
Mike,
I extruded an arc. And then created a sketch for the cut extrude. The sketch is different from what you need but that can be managed.
I would doubt if this is correct as cut on the curve is going straight instead of normal/perpendicular to the surface. So if you need the cut normal/perpendicular to the surface, model this in Sheet metal (again same two features)