Replace face tool vs revolve for arc in model?

I have followed a couple of different watch modeling tutorials. I have learned a lot but also left having some questions.

I am looking for the best approach to creating the end lugs on an angle while having the middle part straight, just like a regular watch. Picture for reference:

The first way I achieved this was through the Replace Face tool to create an arc, however, this creates an arc on the whole piece whereas I need the middle piece straight. This also created a problem where the lug is not flush with the main object.

The second way was modeling the angle on a side profile sketch and using the Revolve tool to create the object. I then Intersected the two. Overall this is closer to what I am looking to achieve, but the lugs are no longer straight and are sideways (when comparing the front view to the first and second method). The middle part is straight and the lugs are now flush with the main body. However, the front lugs should be straight like the first method, but seem to be on an angle,

Am I doing something wrong? If there is another method to achieve the end goal to create the lugs like on a regular watch, please let me know. Thank you!

Hi @Benjamin,
Can it be a solution if you revolve a solid body with a curved bottom over your body? Like the closed profile in this picture:

If you Subtract it from your existing lugs, it will leave a drafted surface all around.

The bottom of the lugs can be created by subtracting a simple extruded body.

If I misunderstood you - which can happen - please highlight the desired shapes on your pictures and we will find a solution.

ps: the bottom of the front and back lugs are not symmetrical on my model

Hi @KPeter_Shapr3D

Thanks for getting back to me. Over the past 10 days, I have been trying different methods, and I am still not able to achieve the look I am looking for. A watch for reference has the lugs slowly tapering down while still fully having a straight edge at the top, like this picture:

As mentioned before, when I create the taper, there is no longer a straight line and is uneven (which is very challenging to manufacture via CNC)

When I use the revolving method and your suggestion method, the straight edge is achieved but the end of the lugs are no longer straight.

I’m trying to achieve the best of both worlds, straight ends on each end with a curve. Basically how every watch looks. Looking forward to your response.

Yeah, I see. If there is no shoulder around the cylindrical body, it can be done with a Loft as on the attached picture, just take care to make the lower points of the cross section (marked with red) horizontal. It can be done by creating a spline on the inner side of the lug then project it to the reference plane on the picture. Please note that the reference plane is placed at the exact place where the curve connects to the cylinder. If you snap the endpoint of the outer spline (nr 2) to the endpoint of the projected spline, it will result in a horizontal lug edge.

In this case, it was really simple to make the cylinder-end of the lug horizontal. If you have a shoulder around it like on some of your pictures, you should make the splines tangent to the shape of the shoulder to create a smooth connection.

Plase see the attached .shapr project file, I hope it helps
watch.shapr (232 KB)

Thanks, @KPeter_Shapr3D

I am still learning and trying to understand so I appreciate your help. I was able to get closer to what I am trying to achieve. A couple of follow up questions.

  1. How were you able to create that plane? I have tried with all the settings but couldn’t replicate what you have.

  2. I select the inner line to the loft to the plane, but I must delete the projected line on the plane for this to work, correct?

  3. After I create the new shape with the Loft tool, I then subtract it from the lug?

  4. With the new lug, I am no longer able to Chamfer the top edge. How can I go about this?

Please disregard my previous reply @KPeter_Shapr3D - I figured how to add the plane correctly to mimic the result you got.

However, I am now facing another issue when using the loft tool then subtracting it from the lug. One side is higher than the other, which becomes uneven from the side profile. Also, when looking at it from the front profile, there is a small dip at the top and not straight. Everything else seems fine, this is now the only problem. How can I have it align correctly so they are both the same height on both sides with a straight top?

Here is a picture of a watch lug that I am trying to model: Screen Shot 2020-11-20 at 3.49.14 AM

Pictures of uneven lugs when using loft/subtract method as suggested.

Wow, great to see the progress and I am happy to see that you have found a solution!
When creating the cross-sections for the loft, you may need to play with the splines. In my attached file I used just 3 control points, which was enough for the demo. What you are looking for is a more refined spline on each plane, which can be achieved by placing more control points and refining the spline to get the result you are looking for.
If the shape is still far from the required result, you can add a construction plane between the existing planes with the Midplane option and define a third cross-section to loft on that plane.

After the lug is ready, just Union the bodies together, and the Chamfer tool will be fine along the edge.