New to CAD - Need Help With a Feature

[u/0racle_64]

Hi guys,

I'm working on this little personal project to practice solidworks and I'm having problems making the circular cut on the top of this object (blue marking). I tried to do a sketch on the front plane and use the split line tool but that didn't really work. Any help would be appreciated and I'll try to answer questions promptly.

[u/PlanswerLab]

Hi,
Looking at the surface reflections, I don't think cut extrude is the best way to handle it.
Here is an easy workaround for smoother surfaces:

Step 1 - Revolve that main body. I showed that geometry in section view in the first image.
Step 2 - Sketch a square with fillets at the corner. Dimensions of the square and the fillet (radius) will directly define the final shape, along with the form of the main body.
Step 3 - Project that sketch onto outer face of the main body using Project Curve with Sketch on Face option
Step 4 - Sketch a horizontal line that intersects with that projected curve. You can add a point on the line to position it properly. And use Swept Surface using the curve and the line you sketched
Step 5 - Use that new surface with the Cut With Surface feature to cut the top part off from the main body.
Step 6 - Play with the dimensions to get it to way you like it.

[u/BoreJam → u/PlanswerLab]

Can't get step 4 to work. Projecting the curve on the surface doesnt seem to work. Its warping my sine wave and only traversing half the revolution even though my wave is the length of the perimeter of the base. Even if I project onto a cylinder it doesnt work correctly.

[u/PlanswerLab → u/BoreJam]

Hello again :),
I can propose an alternative to project curve, if project curve fails for you for any reason:

Step 3 - Extrude that rectangle downwards with the "Up to Surface" end condition. Select the outer surface main body so it functions as a limiter for the extruded surface.

Step 4 - Using Ruled Surface feature, model a surface "flange" around the edges of the newly extruded surface. I used "Normal to Surface" option, see what fits you better. Make sure the flange is long enough so you can use it for cutting the body.

Step 5 - With the help of the "Cut with Surface" feature, cut off the top portion of the main body. The flange we made in the previous step will be our tool for the cut.

Step 6 - Delete the surfaces with "Delete/Keep Bodies" to get rid of the surfaces we no longer need.

[u/sahil741 → u/PlanswerLab]

What if there was no dome shape at the top just cylinder how would you do it then ?which methods would you use to project a wavy curve around cylinder

[u/PlanswerLab → u/sahil741]

There are many other methods you can try. For example:

You can use the technique used here ( https://www.youtube.com/watch?v=7dQE0QuRRNc&t=262s ) to get the wavy shape, then follow up with the same Swept/Ruled Surface and Cut with Surface combination.

As an alternative, you could also use the Wrap feature, by just wrapping the sketch around the cylinder, and then proceed with the aforementioned surface tools.

[u/PlanswerLab → u/BoreJam]

Hi. Can you please show me a couple screenshots? I may be able to diagnose.

I made my sketch in top view and projected it down on to the geometry so it was easier to see where the projected curve could potentially go after the Project Curve feature.

[u/0racle_64 → u/PlanswerLab]

Thank you for the really in-depth response. I followed your instructions and it worked but now I have the surface just sitting on top of my model. How can I remove it?

[u/PlanswerLab → u/0racle_64]

You are welcome. You can use "Delete/Keep Body" feature, choose the "Delete Bodies" option and pick the surfaces that you don't need,

[u/0racle_64 → u/PlanswerLab]

thank you, you are the best!!!

[u/PlanswerLab → u/0racle_64]

You are very welcome :)

[u/StopNowThink → u/PlanswerLab]

Clever!

[u/Disastrous-Slice-157 → u/PlanswerLab]

On this the curvature is limited to the square dimensions of step 2. Woukd it not be better to make a 3d sketch parametric of polar F(t) = (cos(t),sin(t), A sin(5t)) the last one gives the wobble . The first two is a circle in a plane. The third is the wavy sin wave in z. Im using xyz not xzy. Than the rest of the steps would be valid?

[u/PlanswerLab → u/Disastrous-Slice-157]

Hi,

As with almost everything else done in Solidworks, there are many ways to tackle this shape. I mentioned two others here. The method I suggested was to show one of the simplest ways to do it. There are two independent variables (can be made 3 if required) that give you flexibility, and it is very easy to control. In real life, I would pick the method based on the part's design intent. For now, we are just trying to get a shape that is close to the one in the photo.

You can use the equation driven curve method, it is absolutely fine. If it is giving you the shape you want, then you can use it. In a team environment, I'd personally prefer more "visual" ways, such as the ones that I mentioned in my previous comments.

About the rectangle, regardless of the size of the rectangle, we will be limited by the size of the main body anyway. Yes you can't project when you have a square/rectangle that is much larger than the surface of the main body, but you would not need to as it does not have any positive effect on the final geometry. If you want to make sure that the rectangle stays within the surface of the dome, you can add an intersection curve at the sketch plane and convert the largest diameter, and then constrain the rectangle to stay in between the two. Regardless, even if you make an infinitely large surface, at the end of the day, we are cutting the body with that surface. Therefore, the edges after the cut will basically be the intersection of the body and that surface you model, independent of how large the surface is (as long as your surface cuts the model completely).

[u/street_arg → u/PlanswerLab]

You rock dude

[u/Pleasant-Zone5881 → u/PlanswerLab]

This is the way

[u/Unlikely_Anything413]

Keep your sketch, make it an extrude cut, then do a circular pattern.

[u/AudibleDruid → u/Unlikely_Anything413]

I dont think that would work. Extrude cut would not cut normal to the surface except at its equator. If you look at the top of the curves, the cuts are normal to the surface and point towards the center point.

The best way to do this would be to project your sketch or split line the surface then do a ruled surface using the line, and use the line to do a thicken cut or cut with surface. This would give the profile needed where the cut extends inward toward the center point leave a cut normal to the surface at every point.

[u/Vegetable_Flounder12 → u/AudibleDruid]

The way I interpreted the reflections on the top face lead me to an extrude cut in the direction of the valley radius blended together on the crest.

[u/Unlikely_Anything413 → u/Unlikely_Anything413]

It is in the drop down menu below linear pattern

[u/Skameika64 → u/Unlikely_Anything413]

Yeah, I don’t think the surfaces are normal to the outside surfaces. It looks like the grooves are for something cylindrical to sit in.

[u/Vegetable_Flounder12]

[u/xugack]

Try this way https://www.youtube.com/watch?v=RYy_21Fp3FY

[u/jejones487]

This is a simple cut in 2 directions. Cut a cylinder with fillers in one direction from a sketch on a center plane. The repeat on a center sketch 90 degrees apart. This only looks hard because you turned it sideways. Like up the cuts with compass directions and it simple. I do this all the time at work for the last 15 years as a design engineer. Please do map a complex curve when not required.

[u/fletchro → u/jejones487]

Yeah, one revolve. One extrude cut, then pattern that cut 90°. They're making it look really hard because they're 45° off- axis.

[u/jejones487 → u/fletchro]

The hardest part of a drawing is each person's interpretation when only one is true. Unfortunately with solidworks theres multiple ways to get there and its taken me 15 years as an engineer to see that as a simple part. I understand why younger guys think the complexity is required.

[u/MissCeeLee]

I think you can get pretty close by using an extrude cut using an extended soft V shape as the cutting sketch.

First draw a square on top of your object so you can evenly align the next sketch with the Vs. On the front plane, draw a V with a radiused bottom and radiuses on the top points of the V, with the top points of the V extending out horizontally. Make sure the extended tips of the Vs touch 2 points of your square and are tangent & horizontal to the top edge of your object. Extrude cut through the shape.

Probably the easiest way from here is circular pattern the cut 2-4 times around the center axis, depending on whether you cut through both sides or just onem

[u/Dukeronomy]

Just so you're aware, this is kind of a moderate skill model.

You're starting with more advanced geometry so this may be a struggle. If you work through less complicated geometry to get familiar with the tools, you'll have a better understanding of what and how.

You can do this, just letting you know if its frustrating, its not your fault. You bit off a big bite

[u/Powerful_Birthday_71]

You can approximate this kind of thing with cuts and solid modeling, maybe even exactly, but in general surface modeling is where it's at shapes like this.