3 Replies Latest reply on Oct 8, 2014 8:06 PM by Jerry Bentley

    Inventor Slice Graphic command

    Jerry Bentley

      I am an advanced user of Inventor,  I have just purchased Solidworks because I needed some features  Inventor did not offer.   Everything is going well except I can't find a way to slice my part and sketch on the inside of the part.  I need to both be able to sketch on the inside of the part and  treat it like a section view so I can see what I'm doing.  In Inventor I would also project the geometry so I could pick the edges or center points of the area I had sliced  .  I know Solidworks has to have something like this because to me It would be a toy without it.  And I know Solidworks is not a toy. What am I missing?  The only comment I have found is where someone said to use the section view.  I have not found a way to sketch on the cut area of the section view and pick the edges, points and so forth to snap on or use for dimensioning .

        • Re: Inventor Slice Graphic command
          Deepak Gupta

          You can use intersection curve option to get the projection of the selected faces. For this you need to be in sketch mode.

          • Re: Inventor Slice Graphic command
            Jim Wilkinson

            Hi Jerry,


            I'm not completely familiar with Inventor, but if I understand it correctly from what I can find through a Google search, SOLIDWORKS does have equivalent functionality.


            First, SOLIDWORKS has what are called silhouette edges. In the image below, I am sketching on the Front plane which goes down the middle of the part. I can choose the "silhouette edges" which are virtual edges representing the silhouette of the curved faces when looking at the front view. So in the case of a part like this and sketching on a plane down the middle of the part, they are where the plane intersects the curved surfaces. These edges are there when in a sketch or when in a drawing without having to run any extra command to create them. You can select them like any other edge, and the cursor is different so you know it is a silhouette. In this case, you can see I have used the Convert Entities command on 3 of these edges and am just about to select the 4th to use Convert Entities. Note that Convert Entities can be used for edges/entities that lie on the sketch plane as well as those that do not (like the round edge that is perpendicular to sketch plane). Here is the help topic for Convert Entities: 2014 SOLIDWORKS Help - Convert Entities. I believe it is similar to Project Edges in Inventor for this usage.


            If you want to do the above task while looking at the model in half view, simply turn on the section view using the Front Plane as the sectioning plane. The section plane has an option to either just cut the graphics or it can also "virtually" cut the model so you can measure edges, etc. Note that these edges cannot be used for reference in commands like Convert Entities because there is no feature stored in the tree for the section view to know where the section view is defined. In this case, you need to use the "Graphics-only section" option and then you can select the silhouette edges and use Convert Entities like above. If you don't have Graphics-only section turned on, then the "virtual edges" from the section view get in the way of picking the silhouette edges. Below is an image of the same process with the section view on:


            Now, let's say your sketch plane does not go down the center of the part. In that case, instead of being able to select silhouette edges, you need to get an edge at the intersection of the face and the sketch plane. In Inventor, this looks to be called Project Cut Edges and you have to be in Slice Graphics mode to use it. In SOLIDWORKS, as Deepak says, there is a command called Intersection Curve. Here is the help topic for it:  2014 SOLIDWORKS Help - Intersection Curves. It is actually much more powerful and can do many more types of intersections than this particular task. As shown below, I have created the intersection between 3 of the 4 faces and am just about to pick the fourth face to create intersection curves for it. If the surface intersects the sketch plane multiple times, it will create multiple intersection curves (see that it created them both on the top and bottom in the image below) but you can delete the ones you don't want.


            As with silhouettes and convert entities, intersection curves can be made with or without the section view turned on as shown below:



            I hope this helps,