[DCogswell]

I design a lot of "turned" or round parts that are made on mill/turn type machines. When making a component in SW, should I be using "extruded boss/base" or using "revolved"?

[fpd56]

It's fully depends on the shape and profile.
If you have any complicated part, you can post here to get the help and advice.

Thanks

[DCogswell]

I wouldn't consider them that complicated, I'm just looking for a general starting point from people that have a lot of experience using SW.

I haven't had a chance to go thru training, we just got an additional seat for myself so, I've been doing a lot of self-training via tutorials & whatever I can find on youtube.

How do you move the "top plane"? I saw where someone selected the top plane and moved it to the "surface" of the extruded boss (diameter) then selected that surface to do an extruded cut.

I'm trying to make a round tool holder that would hold onto a round carbide drill. So, the geometries are simple but, I want to add a cross hole & thread for a set-screw to clamp onto the drill.

[broby]

Hi,
Generally speaking I usually will pick a revolved profile every time when modelling a "shaft" type of profile.
Sure you can build up the exact same profile by building up a series of extruded shapes, but that would be a PITA!
Also, should you want to model in "undercuts", I would consider the fact that a revolved shape would allow this to happen much easier than a "stacked" series of extruded shapes.
As for the other question re moving the top plane...
First thing you need to understand is that the three basic planes are unmoveable. What you probably saw was that someone had selected the plane and then, Holding down the "Crtl" key, dragged a "Copy" of the plane to a new position.
Setting the new plane on the surface of the curved face can be done by ctrl dragging a suitable plane somewhere close to the surface you want, then, select the "Second Reference" box and select the surface you want the plane to anchor to. You may see the plane flip 90° at this stage, if you do, press the "Parallel" button in the "First Reference" section. The new plane should now be located on the surface of the desired diameter, thus if you change the diameter, the plane will follow to the new position.
Please keep in mind that this is only ONE possible way of doing this!
for e.g. you could just dimension the position of the plane parallel to the original plane, and link the dim to the diameter, or draw a line that has it's length driven by the diameter of the shaft and sit the plane on the end of that line... or or or ... so many different ways of doing things in SW that it can be a tad confusing at times.
Good luck and stick with it, Solidworks is a great program.
Cheers
Brian.

[JerryFlyGuy]

A good general rule of thumb is to model in the same way a part is made. If the part is turned to shape then it's recommended to model it in a revolve.

The same thing goes for secondary operations. If a pc of material is welded into a structure and then machined in the assembly it should be modeled that way w/ cuts at the assembly level.

To every 'rule' [or recommendation in this case] there are exceptions. I try and follow this where possible and it's rarely let me down to date [9yrs later...]

Fwiw

[mattpatt]

I design a few shafts here and there and these days I mostly sketch the outline and then revolve it. With all the dimensions in the sketch it's very quick and easy to change things.

[T D]

I would model the parts with design intent in mind.
If you have similar part numbers / configurations, model in a way that the features can be easily suppressed or changed as needed.
If there are features that are commonly revised I would give them their own feature in the tree.

Here is what i would do if I had a shaft with two different diameters with a fillet as a transition.

1. Revolve the profile without sketch fillets
2. Use the fillet command to generate the needed fillet

This allows you to make a configurations or revisions with or without fillets, and or different diameters shafts.