swept boss option greyed out
swept boss option greyed out
(OP)
I'm trying to do a swept boss and have created the path and profile.

Here are a couple jpgs of the layout. I'm sure my path plane is perpendicular to the profile plane. However the option for swept boss is greyed out? Can someone help out on this?


Here are a couple jpgs of the layout. I'm sure my path plane is perpendicular to the profile plane. However the option for swept boss is greyed out? Can someone help out on this?






RE: swept boss option greyed out
Try that out and see if it works.
Jeff Mowry
www.industrialdesignhaus.com
A people governed by fear cannot value freedom.
RE: swept boss option greyed out
Jeff Mirisola, CSWE
My Blog
RE: swept boss option greyed out
This is an assembly. You need to be editing a new part in the context of the assembly. There are only a few features you can add at an assembly level and most of them are cuts or welds.
- - -Updraft
RE: swept boss option greyed out
Jeff Mirisola, CSWE
My Blog
RE: swept boss option greyed out
RE: swept boss option greyed out
Jeff Mirisola, CSWE
My Blog
RE: swept boss option greyed out
From your comments it seems as though you might be pretty new to SolidWorks. For one you mention swept cut when you should be making a solid so it would be a swept boss, not a cut. Your other comment "Also I don't know how to create this in anything but assembly, not sure if there is another option?" indicates a lot as well. An assembly is an assembly of parts and not an environment to create new parts per se. You have a parts environment and then an assembly environment to put those parts together.
We are all too happy to assist you, but it appears you would dramatically shorten your learning curve if you were to go through the SolidWorks tutorials (go to Help -> SOLIDWORKS Tutorials).
- - -Updraft
RE: swept boss option greyed out
RE: swept boss option greyed out
- - -Updraft
RE: swept boss option greyed out
SW is absolutely great but for the person, who does not continuously dedicate his whole working day on learning and using it but needs it as a secondary tool the non-expert-unfriendly help makes it too complicated. And that is a big market that with little effort could be accessed. It is not the programme that is presents the complication, but the difficulty of the experts to understand the problems of the lesser-experienced person's, who does not want/need to work with all the bells and whistles.
RE: swept boss option greyed out
E. Morel
M.E.
RE: swept boss option greyed out
1) I made a quick assembly consisting of two tubing connections, mated where I wanted them to be for this example (5 inches apart vertically and horizontally, but sharing a center plane). See Image ASSY1.
2) Select Insert >> Component >> New Part. Click in empty space on the screen. This adds a new part to your assembly tree. Right click the new part, click "Rename" and name it something you want, I named mine "TUBING". Right click again and "Save Part (in external file)" and select where to save the model. See image ASSY2.
3) Right click the new part and click "Edit Part" to being editing the new component. Your existing parts in the assembly will go transparent. I like to turn on any sketches from existing components in the assembly that I can use as reference lines. In this case, I turned the sketches on visible for both tubing connections. See image ASSY3.
4) Start a new sketch on whatever plane is your aligned center for both parts. In order to use the existing sketches as reference, I like to use the Convert Entities tool to make the sketches usable relations in the current sketch. In this case, I used the Convert Entities tool and selected the center lines of both tubing connections. This makes them usable lines in my new sketch. See image ASSY4.
5) Now, on the center plane I draw my sweep path that I want my tubing to take, mating it to the converted center lines from the other two parts. See image ASSY5.
6) Now I sketch the profile on the plane that I want, ensuring the center point of my profile is on the path line. See image ASSY6.
7) Now I simply use the Swept Boss tool to make the sweep. See image ASSY7.
8) Once complete, exit the part editing mode just like you would edit the sketch. See ASSY8.
The good thing about this, is that if I change the distances of the tubing connections and where they are mated, the tubing will automatically update and follow, since I mated the sketch to those two parts.
-E
M.E.
RE: swept boss option greyed out
I was able to create this tubing in part mode after I laid it out in assembly. I was certain I was able to do this in assembly in the past but I was probably thinking ProEngineer. However after reading Emorel22’s post it looks like it can be done in SW as well. I will review Emorel’s post in detail as I know this will come up again.
Thanks for the help!