Why is it you have create another center line typ in order to dimension a dia in sketch? Why cant you just use the line you have on center all ready? or change it to center line and still have it part of the profile?
Why is it you have create another center line typ in order to dimension a dia in sketch? Why cant you just use the line you have on center all ready? or change it to center line and still have it part of the profile?
Can be whatever you want it - you need a construction line, then right click and select this
I guess this more of a statement of why is it this way. John Stoltzfus I understand that but, it doesn't work for what I'm looking for. Just weird how you have to draw another line to get your symmetric dimension option. O well..:)
Technically you can change the first line you drew into a Construction line and put relations to it and then turn it back into a "solid" line. If you add a symmetric dimension (diameter) to it it will revert back to the single (radius) dimension. I do agree that the way that this behaves is odd.
It can be a centerline and that's how most of us were taught. In SW2015 and prior the centerline had to be there so the software understood what to revolve around AND you would be able to dimension the full diameters as you have above.
Now, you don't need the centerline (I think, since I'm not in SW2016) to do the revolve.
I like having it there but I'm old fashion.
Steve C
Well I'm new and where I come from you made that you axis and you could then dimension to it. No extra lines. Where I work now they all put a center line there as a habit. I just have to get use to it this way
I do what Tony Cantrell mentioned. Create the line at the center of the revolve as centerline type so you can dimension across it. Close the sketch. When you select the sketch for a Revolve you'll get the message below. Click "Yes" and move on. There's no need to create an extra line. (By the way, if anyone from SolidWorks sees this, I'd really like a "Don't ask me again, ever" check box on this message.)
Not me, Glenn. Sometimes there maybe several non-solid lines so I'd like to have the question there so I make sure i'm getting the correct revolve.
Steve C
Steve Calvert wrote:
Not me, Glenn. Sometimes there maybe several non-solid lines so I'd like to have the question there so I make sure i'm getting the correct revolve.
Steve C
I understand. Then when you got the message you wouldn't click the "Don't ask me again" box.
ok, I was doing a sketch within the command. It acts different than if you do a sketch first then choose Revolved Boss/Bass. But to sum up, you have to draw a center line no matter what. Do you want it sticking out so you can see it? Or under a line where you cant see it?
Todd Bush wrote:
But to sum up, you have to draw a center line no matter what. Do you want it sticking out so you can see it? Or under a line where you cant see it?
I'd have the extension line extending past the solid line. I'd never intentionally have one line hidden behind another one. That could cause all kinds of confusion when you go back to edit and don't remember what you did (or if someone else edits the Part).
I did notice that SW 2016 when I created my centerline and did my dimensioning everything looks fine. When I did my revolve you do get the "sketch is open" message and SW will add an additional line to the sketch..shaking my head on that one..you are telling me the modeler can't figure this out without a closed sketch...anyway when I went back in to view the sketch I have two lines. But to give SW some credit they do extend the centerline on one end for you so that they are not fully overlapped.
You're right. I'd never noticed that SW adds a second solid line on top of the construction line. I had always assumed that it turned the construction line into a solid one. It looks like I learned something today.,
Todd Bush Because the sketcher is a primitive sketcher tool.
Your question runs really deep into the history of sketchers and the 2D rules written into the sketcher code. Rules like linear lines can only provide, horz, vert or aligned dimensional constraints. To resolve this you need to create a centerline "special" line type to override the existing rules and apply diameter values/settings to a dimension.
I feel your pain. I'm used to being able to pick the diameter dimension and go to town. Then pick my axis of revolution which could be a non-sketch line, a datum axis, defined axis using two points, etc. Ahhh...the good ole days. Oh, and I did have the ability to turn on create solid or sheet body at the time of create too!
Thanks all for your answers. Looks like there's two different way's. It just depends on which way you sketch.
What's the most common way to sketch? In the command? Before the command? I come from where you sketch in the command. So that habit for me.
Another reason why I do it with a centerline is because I find myself changing the revolve and adding a hle later in the design and with the centerline already there I can just add a solid line that would create the revolved hole without too many distractions in the initial sketch.
Steve C
Just another reason you should be able to use a datum axis or be able to define the axis outside of the sketch! I recall doing this with NX many years ago. Since the datum axis is the intersection of planar geometry (surface (finite) or datum plane (infinite) and other geometry the location is driven by the geometry and not some dimension buried inside a sketch. That allows you to locate and moves things around quite easily (components, features and construction geometry). Ah the good ole days!
Todd Bush I would go with creating the centerline inside the sketch environment, like Steve mentions, and then build the rest of the profile (it will be open) and then allow the system to generate the "unnecessary" geometry to close the profile when completing the feature. This allows you the most flexibility and the ability to use the full diameter dimensions/parameters.
The centr line gives you the symmetric dimension option. The line you point to could be a center line if you are doing a revolve and say yes to close profile.