How to revolve Boss / Cut with offset angle from drawing plane

[Super169]

I have a base body created by a revolved boss from a curve. I need to add something parallel to the body surface. How can I achieve this using revolved boss/cut with an offset angle? Can I directly convert the original curve to a new plane when creating one?

Below is a simple example to demonstrate what I'm looking for.

1. the base body was created with revolved boss from a curve in front plane
2. need to cut a window from 30° to 60°
3. need to add something parallel to the body from 45° to 70°
......

What I can do for 2 & 3
2a. create a plane at 30°
2b. create a sketch on this plane, use convert entity to get the body shape, then draw the window
In this example, it may just draw a rectangle covert the body, but something we need to have the exact shape - e.g., add a new body as the glass of windows.
2c. revolved cut for 30°

3a. create a plane at 45°
3b. create a sketch on this plane, use convert entity to get the body shape, then the required shape
3c. revolved boss for 25°

In here, the convert entity sometimes does not work if other operation already done on the body.
For example, after 2, the convert entity cannot get the full curve as part of the curve is missing.

I would like to know if there has better way to have revolved boss / cut, starting with offset angle, so that I can make all sketch from original plane.

Or when I created a new plane, how can I convert the original curve to the new plane? The convert entity of original sketch will just project the curve on this plane, which is not rotate to match the plane.

[matt]

I'd be willing to bet that you have a way of doing this in some other CAD and you're trying to recreate that method.

I really don't understand your description. "30 degrees" from what?

I'm guessing you're trying to recreate the indented window in the example. I would draw a pair of lines on the top plane. The lines meet at the vertical axis of the revolve, and are drawn at the angle from one another that you want. Then extrude the lines AS A SURFACE BODY in the area where you want the window. The use the OFFSET SURFACE to offset the surface of the revolved solid. Then trim the surfaces and keep the parts that make the walls of the inset window. Then use CUT WITH SURFACE to cut the solid with the trimmed surface.

There are other ways - draw the angled lines as above, but use SPLIT LINE, and then do the same for the top and bottom of the window to split out a rectangular area on the revolved solid. Then use the fancy technique of extruding the surface area inside the split lines with the extrude command.

You're probably having difficulty using the "convert entity" command because you have to grab a silhouette line. It's finicky anyway. Lots of ways to do what I'm imagining you're asking, but it's not really clear to me what you're asking.

[Super169]

It's not easy for me to describe what I'm looking for.

I hope that I can explain in a simple case below,

a. The main body of this 3D model is generated by a specific curve revolving around the Z-axis.
b. At a specific position(30 degree from drawing plane), a 30-degree window is cut along the outer wall.
c. At a specific position(45 degree from drawing plane, a small piece protrudes from the outer wall, with a width of 25 degrees.

What I have to do now:

1. Draw the curve in front plane (sketch A)

Revolve boss around Z-axis to create the main body

2. Draw two lines with the required angle at starting position for b & c (i.e. 30 & 45 degree)

3. Create a plane based on 30 degree line

use convert entity to get the body shape at this angle

draw the windows shape (sketch B), then revolve cut for 30 degree

4. Create a plane based on 45 degree line

use convert entity to get the outer shape

This time, it cannot get the full curse of main body as the part of it has been cutted before


Use offset entity to get the outer curve and complete the shape (sketch C), then use revolve boss to add the protudes part.

In here, I have to create two extra planes and convert entity to get the body shape, sometimes convert entity from body may not get the full shape. In the real project, I need to create another body to make sure I can get the shape in the plane from any angle. But it still need to create many plane in different angle in order to start the revolve operation.

For b & c, if I can create the sketch B / C in front plane as sketch A, then revolve cut with sketch B starting from 30, end at 60, and revolve boss with sketch C starting from 45 and ended at 70. I can use sketch A as reference directly.

But now, it can only specify the angle to revolve, and must start from the drawing plane. Or I have to make a revolve boss x angle then revole cut y angle to similiar revolve from y to x.

I would like to know if there has a better way to create such body (the actual case may have many revolve cut & boss based on the body shape).

Besdies, in this example, when I use covert entity to get the shape, it will miss the top part as a windows is cutted.
I would like to know if there has any way to revolve sketch A, instead of use convert entity from main body.


Below is a sample project which has many steps with a sketch based on the original curve, but starting in different a plane rotated with some anlge from the orginial drawing plane. A revolve boss / cut with starting angle may reduce much dummy steps.

[matt]

Your method takes a lot of steps, and it relies on methods I would consider unreliable - like the convert entities from a silhouette edge and face-to-face contact for non analytical surfaces.

There are several ways you might do it:
1) make your initial shape however you make it, then make the inset window by extruding those 30 degree lines as a V-shaped surface body. Make lines for the top and bottom of the inset, and extrude as surfaces. Then trim the two extruded surfaces up so you have a neat little box. Use the surface box first to cut the solid, then to thicken, adding the inset box to the part.

2) Draw a rectangle, use split line on the face of the part, then use special functions in the Extrude command to push the inset window. Alternately you could use Indent, but you need a solid body tool to do that.

3) Use 3D sketch to sketch window edges directly on the shape, then either split the face and use 2) above or use the tricky extrude commands to make either then inset or the outset.

4) Use offset surfaces and extruded surfaces to make the box.

Revolved cuts of line-on-line converted entities can cause funky errors.

I don't have the software installed right here, but once you see the other non-sketch based methods to do this, it opens up a new world for you.

[Super169]

Thank you very much for your reply. Yes, you have point out the reason why I ask for other options even I can already make it, I also find the convert entities is not reliable especially for such conversion from the intersection between plane and body, subsequent operation may have unexpected result.

I am watching YouTube to learn SolidWorks, and I only understand a fraction of the commands. I will try to study the methods you provide, but I am not familiar with surface operations and cannot fully comprehend them at the moment. I hope to learn some non-sketch based skill from them. Thank you very much for your help.

[Glenn Schroeder]

. . . I am watching YouTube to learn SolidWorks, and I only understand a fraction of the commands. I will try to study the methods you provide, but I am not familiar with surface operations and cannot fully comprehend them at the moment. I hope to learn some non-sketch based skill from them. Thank you very much for your help.

I would advise caution with that. If you stick to the ones produced by the VAR's you should be fine, but there are some individuals out there posting videos who don't know as much about Solidworks as they think they do. You can learn some bad habits if you follow those.

[Frederick_Law]

You're thinking too much.
You cut from same plane of the sketch.
One profile to cut top small window.
Another to cut bottom.
Then array them.
Technically the cut don't need to use the curve. It can be rectangle.
Try it.

[Super169]

Thanks for your reply. I just try to simplify the case in the question, so it can be done by a larger shape, and it may start from any position.
In the real situation, the shape is not as simple as this, and such oversize shape can only work for cutting, if it need to filll with a new body (e.g. add a glass in place), it need to use the exact shape (I just try to make a simple example, and I know that in this example, it can create from original curve then move it for create the glass).
And the button part is a boss operation, the shape need to align with the body, it can't be done by a rectangle.
In fact, both situation are similiar, which need to get the original curve for revolve boss / cut.

But I'm not sure if I have missed a point in your suggestion, what does it mean by "Then array them." ? Does it mean I can retate the operation to target position, similiar to shifting the starting postion to target angle. Or use the circular pattern for them, I've also doing this for some repeated operation (e.g. if cutting two windows of same size in different angle), but the circular pattern seems cannot remove the original one, so I still need to start from the new plane.

[CarrieIves]

Have you tried using the main revolved sketch as a derived sketch on your plane that is at your angle?

[Frederick_Law]

But I'm not sure if I have missed a point in your suggestion, what does it mean by "Then array them." ? Does it mean I can retate the operation to target position, similiar to shifting the starting postion to target angle. Or use the circular pattern for them, I've also doing this for some repeated operation (e.g. if cutting two windows of same size in different angle), but the circular pattern seems cannot remove the original one, so I still need to start from the new plane.

You cannot remove first "instance" in pattern.
So you need to create it at correct location relative to other cut out.

There are 3 operations: Boss, Cut and Intersect.
Use rectangle to Intersect instead of Cut the body will give you the "glass".

Maybe easier to Cut with solid body.
Can't pattern sketch but solid can be patterned.

[len_1962]

Here is a part that I did using multple bodies, boss extrudes with offset possitioning, circular pattern bodies, combine tool add and subtract picking just the bodies I want, replace face from offset surface. I think using simple extrudes a solid feature of patterning and combine feature make powerful tools and easy to ge cool results.

used a total of 2 sketchs and didn't have to create any new planes. used front plane for revole and top face for the angles aka slices of pie.

rollback and watch what I did.

i've included the file.

[Super169]

Here is a part that I did using multple bodies, boss extrudes with offset possitioning, circular pattern bodies, combine tool add and subtract picking just the bodies I want, replace face from offset surface. I think using simple extrudes a solid feature of patterning and combine feature make powerful tools and easy to ge cool results.

Thank you very much for your help.

I am studying the file you provided, and I can understand most of the steps except for 'Replace Face1.' I have never learned this command before, I guess it is similiar to cutting the body by surface, I can only use split command before, and I learn this command now.
In fact, I am not familiar with commands related to surfaces. For now, I have only learned how to create bosses or cuts from sketches.
I should try learn surface commands more seriously.

However, in many projects, it may still need to add different bodies align with the oiginal curve.

For example, the glass and frame of the windows in cable car project as below,

To ensure proper 3D printing, a small gap need to be added between the glass and the window. Additionally, a thin sheet will be added to secure the glass onto the main body.

The glass will be as below,

The glass will be installed onto the main body using adhesive as below.

Currently, as this is additional parts, I can make them in original drawing plane as a new body, then use the move/copy command to rotate them to expected position, then combine with main body if needed. And I'd like to know if there has any better option on it.

It may be challenging for me to use binary operations to create the glass after the window is made. Furthermore, a body curve is needed to create the frame. I will attempt to follow your instructions and create them accordingly.

[Super169]

Have you tried using the main revolved sketch as a derived sketch on your plane that is at your angle?

Many thanks.

After google the command "derived sketch", it seems that it create a rotated curve as expected (but seems mirrored, as the object is mainly symatric, I created a half body at begining, and it goes to the other side).
And it seems that I cannot modify the derived sketch directly, and I have to create another sketch by "convert entities and mirror", then create the sketch on it.
But it can give me a more precise copy from the original one, and no need to worry if the curve has been modified by previous commands.

Is it a common way to copy the sketch using derived sketch?

[Super169]

There is one thing that is not clear in my example. The revolved boss result may not always be connected to the main body, such as the door of the cable car. It should have a shape with a small gap from the main body, which is achieved by rotating the following sketch by 25 degrees in my current design.

Using an offset from the original curve would be simpler for me as I am unsure how to use the "replace face" command. I may opt to use the "split by surface" command instead. I am interested in learning various options, particularly surface operations. I recently watched the YouTube video on surface-related topics, and it seems that surfaces can be very helpful in creating complex bodies.

[CarrieIves]

Many thanks.

After google the command "derived sketch", it seems that it create a rotated curve as expected (but seems mirrored, as the object is mainly symatric, I created a half body at begining, and it goes to the other side).
And it seems that I cannot modify the derived sketch directly, and I have to create another sketch by "convert entities and mirror", then create the sketch on it.
But it can give me a more precise copy from the original one, and no need to worry if the curve has been modified by previous commands.

Is it a common way to copy the sketch using derived sketch?

Usually, I use derived sketch for sketches that should be the same. I think you may be able to flip the direction of your plane you are putting the derived sketch on to keep from having to do that mirror. I think your approach with adding another sketch that has the mirrored sketch in it can work. Keep in mind, that splines can get picky about not being an exact mirror.

Not knowing exactly what you are trying to do, I would try things based more on surfaces and bodies.

[len_1962]

Super169,

Well you have alot of questions which makes me think you are fairly green and haven't used many of the things I would use to create your part file.
I have been using SW as a model maker\prototype machinist\SW abuser since SW97+ and have taught both at the SW VAR and colleges.

Here is what I can give you advice on, take what I've given you and then you'll have to expand by trial and error, watching vids from others and take that and use the tips\tricks to accomplish what you need.

Multiple body parts is kind of an pain, you really need to think of the process of what should be first and what should be added down the road as some features get absorbed and other can be used throughout the process of creating the part. seat time is the thing that helps figure out this as thing can blow up and learning how to fix and rebuild come with experience. not really what you want to hear I know but has to be said.

Everyone see's the way to do this differently hence the slew ways to approach this. mine is more of how an Idustrial Designer would aproach it.

you part has many facets that would use a mulitude of features and techincs to get it done. Long way may be your best since you seem to be starting out, that way you understane how and why things are happening and can easily modify and fix errors. My way is more itermedate\advanced do to my experience making parts for ID\models and prototypes.

best

lenny

[len_1962]

Is this just for 3D printing and not an actual production part?

I ask because I whould aproach this different just to save time.

[Krzysztof Szpakowski]

Is it good way?

Part1.SLDPRT

(537 KiB) Downloaded 106 times

EDIT
I'm sorry, but it was late yesterday and I didn't understand your problem. I think that your approach to the topic will cause further problems, such as counter-angles in the side walls of the holes and splines. They will be a big problem when producing a detail on an injection molding machine. Pasting the window is a problem even with 3D printing. you want to glue the windows from the center and the sides of the walls also meet radially to the center. Therefore, there will inevitably be unnecessarily large gaps. In my opinion, it is best to cut out the windows using extrude. from a symmetric plane, or use Draft tools that will correct the problem of opposite angles. Splines from the railway use a dividing line with a wedge to maintain the desired shape on the round surface and then an extractor with a slide away from the surface.

klein00.SLDPRT

(292 KiB) Downloaded 97 times