Hello guys, I am pretty new here. I am trying to do something like this:
It's from Autodesk WikiHelp: Link
Under Sweep Features
I am using Inventor 2013. Everytime the Sweep dialogue box will automatically choose the closed path as profile. When I try to choose the real feature sketch, it doesn't allow me.
I have found several posts here about the same issue since Inventor 2012. Someone said it was about constrain. Others said it's about snap to the point. Some even said it doesn't work with closed path.
This is a pretty basic function, how come it's so complicated? I even tried evolve, but it doesn't accept anything other than circle as default sweep path, if you think it that way.
So could you please help me take a look at my file? I deeply appreciate your help.
Hi, GlennChun, thank you for your reply.
As a matter of fact, in another post of yours, which I can confirm that, Inventor works fine with two closed sketches, one as profile, one as path.
But when it comes to the closed sketch as path, and open sketch as profile, it becomes problematic.
In my case, I used the wrong name. I am actually trying to use "open path" as profile, and "sketch3" as path.
Besides, "open path" as profile plus "Profile" as path works out just fine.
Sorry for the confusing names. My bad. :-)
I am actually trying to use "open path" as profile, and "sketch3" as path.
There are two issues here: Modeling issue and UI issue.
When the path is closed and not tangent-continuous, the profile must be on the miter plane to make sweep work. This is a legacy restriction in ASM (geometric modeling kernel), and this restriction has been removed from ASM. Until Inventor adopts the new ASM, please use the following steps:
1. Create a miter plane:
2. Project the original profile to onto the miter plane:
3. Sweep the new profile along the path:
See the sweep result in the attached closed path sweep B.ipt. When Inventor uses the new ASM in the future, Inventor users should be able to use the original profile perpendicular to the path (i.e., no need to place the profile on the miter plane anymore).
Since Inventor always auto-selects a closed region as profile, you need to deselect the auto-selected entities by using the Ctrl key. Try the following steps:
1. Open closed path sweep A.ipt in Inventor 2013.
2. Invoke the Sweep command.
(You will see the rectangle and the arc being auto-selected as profile and path, respectively).
3. Press the Surface button in the dialog.
4. Press the Profile button in the dialog.
5. While pressing the Ctrl key, select the rectangle and the arc.
(Ignore any pop-up message by hitting OK).
6. Press the Profile button in the dialog.
7. Select the arc.
8. Select the rectangle.
9. Hit OK in the dialog. A sweep surface should be created successfully.
I will talk to the Inventor product designer about the above UI issue.
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register