Our #TechTip this week is by Training Manager John Setzer. Learn how to easily delete a face from a solid or surface body when modeling in SOLIDWORKS.
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Hi and welcome to another GSC tech tip. Today we’re going to take a look at a command called ‘delete face.’ And what delete face does is it will remove a face from a solid or surface body. And then, what we’re left with depends on the geometry that’s involved, as well as some of the options that we’ll explore.
Finding the Delete Face Command
So let’s first find out how to find the delete face command. You can find it by going to the menu, insert face, delete. You can also customize your command manager, just right click and bring up your direct adding toolbar, and you’ll find the delete face there. You can go ahead and run that command. Let’s take a look at some of the options that we have.
First of all, you’re going to be selecting one or more faces to remove from your body. Yeah. And as I do this, I’ll be able to pick a face such as this one or three faces or de-select them and go back to the one from our selection boxes, adding or subtracting faces from that selection set. In the options area, we have three options, delete, delete and patch and delete and fill. Let’s go with just straight delete and with selected face, accept it, and we can see what we have as a result. So face has been removed from our solid body, which means it’s not a solid body anymore. It no longer encloses the volume. You can see as they rotate, you can see the quote inside of the model.
Again, that’s because, well, there is no inside, outside definition for volume. We just have a surface body, no longer closing of volume. You’ll note that the edge color. Where the gap is is blue, because blue indicates the end of the world, if you will, for a surface body. So that’s where our gap is. As we see inside that face is removed.
It’s now a surface body. Let’s edit the delete face feature that we just added and take a look into deleting patch, what delete and patch does, is it well removes the face selected certainly, and then it keeps the solid body definition. By extending existing surfaces or faces to put patch over the gap. The results in this situation would be, as we see these three faces extend to fill what was the left or the gap here I left behind by the remove face.
If I were to edit that feature and pick all four of these faces, deleted and patch. This would be the result as the planar face is simply extending each other. Basically making this a block again, delete and fill, I’m going to right click clear selections and then simply pick this face again and we’ll do delete and fill and there’s an option under, do they even feel for tangent. Or not, um, to delete and fill, well, what’s that’s gonna do is remove the face or faces, that you selected and replace it with one new face.
And that new face can be calculated to be tangent to every edge that the new face is connecting to or simply be connected and not necessarily worried about being tangent. If I say delete and fill without tangency. And we examined the results. It doesn’t look like much has changed, but if I moved to this position, you can see how this has flattened out because the new face that was created in place of the old face does not have a tangent condition to these other faces at these edges where they meet.
Simply put something there, make a new surface in that spot, but just worry about being connected. Don’t worry about being tangent or smooth. If I were to edit the delete face. And put tangency in. Well then it looks like the face was never really deleted, but in fact, it was, this face was deleted and then a new face is putting in its place.
It’s exactly like the previous one. It wouldn’t be much of a point to it and this particular situation, but if I edit the delete face and I pick these other three faces to go along with it, and we do this delete and fill, I’m going to turn off the tangent fill for this. Then we’ll see the results. Well that operation, so four faces removed left with one single face, which is curvature, continuous spline based, but there’s no tangency control.
So this face is not necessarily tangent to this face at this edge or at this edge. Certainly wouldn’t be at this, this face, at that edge. If I did turn on tangent fell for this. I’d get a pretty funky looking surface because what’s happening is this face is being calculated to be tangent to this face at this common edge.
So kind of pulls it in and pulls it back out, kind of swoops it out so that there is tangent to see on the inside portion, not what we would want here, but it does show, it does show how the different options affect the results with the delayed phase come in.
Use Cases / Scenarios
So where might we use the delete face command? Well, it’s actually a really good tool for cleaning up things. In this scenario, I have a model where I have used the, fill command and some setback options to create a blended area where there was once a sharp corner. However, in order to create the geometry that I wanted, SOLIDWORKS had to break this up into a bunch of small faces.
I’d prefer this be one single face curvature continuous across that whole area. The delete face is going to help me clean that up. I’m going to use my delete face command, set my parameters to be deleted and fill because I want a new face created where these several faces would be removed. And I do want tangency as well.
I want my new face to be tangent to the other faces that connects to at common edges. Let’s go ahead and pick you small faces that I would like to get rid of and with the delete and fill and tangent fill options selected, finish up and there we go. A single new face. In place as several other faces that used to be there, and this new face has been set up, so it’s tangent to the other face as it connects to at these three common edges or those sets, and I want it to, I can do it for the other side, or I can even expand this.
I could include these three faces and get a larger surface, across a larger area can curvature continuous. All the way to these edges here and here and here, or go across to the other side and move this guy and these faces and a bunch of other faces.
And then I would end up with one single curvature, continuous face that is tangent to all the other faces. It meets at common edge sets. Yeah. That’s a much cleaner model and much nicer geometry to work with. Here’s another example of using delete phase to clean up our geometry. I have a thin wall part and revolve feature that by its nature extends out through my thin wall because of the sizes involved.
Now, I don’t want these three faces that came through from the other side that revolve feature. People might decide to try and do some kind of a cutaway or like a loft cut or revolve cut or some other kind of thing to get rid of that geometry. But it’s actually a much simpler solution if you use the delete face function.
In this case, I’m going to use the delete face. I’m going to set it to be deleted patch this time cause I want to extend existing surface geometry over what would be the gap. I’ll go ahead and remove these three faces. One, two, three, accept it and the job is done. Nice and simple. Again, I used delete and patch because I wanted to extend the existing surface, which really surrounds what would be a gap there to create the geometry, I want it without having to resort to a new quote patch phase. If I had done or fill phase, but I had done a delete and fill, then there would be a new face separated from the other. I don’t want that. I just want delete the patch, extend over. What would have been a gap if I had just not done either of those.
And so here you can see another example of using the delete face command to help clean up model geometry. It doesn’t matter if this geometry is made in SOLIDWORKS or imported from some other CAD system. This is directly editing. We’re taking existing faces, removing them, and then deciding what to do about the gap.
If we do anything with some of the options that we have here. I hope you enjoyed this little discussion about the delete face command and hopefully you can find use for it. In some of your everyday solid modeling. Thanks and see you next time.
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