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Specifying holes is very common in SolidWorks. If you use the hole wizard to create the holes originally, then you're in luck. The software will help you call out the holes as well. If not we can still specify the holes with simple note changes. In this drawing here you can see we have a few different holes we want to call out, and I can use the regular dimensioning tool on any one of these holes. I'm going to zoom in here, I'm just going to choose this outside edge, and I can add a dimension pretty easily. Notice it automatically adds the diameter symbol and the size. And that's great. However, notice this hole's got a little bit more detail in it than just that.
So that's where the hole callout comes in. So I come up here to Annotations. Notice I've got this thing called the Hole Callout. Click on that and then go here and choose this hole here, and actually it goes ahead and pulls all the data from the Hole Wizard that was used to create this hole originally. And not only does it call out the amount of holes you have, it calls out the diameter of the through hole, it calls out a counter sink, it calls out the size as well as the angle. So that's great. It pulls all that in for me, and I can delete this other one over here, the hole callout does a much better job using holes and also tells you the depth and everything else about that hole.
So, it's a great, great tool for using and working with holes, and it brings all that data from the part and from the hole wizard into this drawing here. Okay, next I can take a look at some of these holes over here. I I use a hole callout on this one here, I can specify, this hole here you can see I've got a through hole I've got another counter bore, I have a counter sink at the top, just break that top edge looking pretty good, but what I don't see here is this hole actually intersects with another hole so I have not fully defined. What's going on with this hole here. So first, let's go ahead an make another view.
So I'm going to click on this, part here. Go over to view layout. I'm going to click on projected view. An I'm going to, drop a view over here on the left side of the part, as well as, another one up here above the part. So now I've got a couple different views, showing that yeah, there is a hole up here, that's going to be intersecting with these holes here. And we needed to find that a little further. So on the basic side of things here, and come back to annotation, click on, Hole Callout, and just call out this hole here. Great. Now over here, I can see, if I change the view, instead of the hidden lines removed, let's go ahead and click on Hidden Lines Visible.
And you can see actually, there's a lot going on behind the scenes here. All these hole are actually intersecting. But that's a little bit complicated in Difficult to see really what's going on here because you can see these other holes behind the scenes and they're all intersecting together, so it's really not very clear what's going on. So instead of doing that, let's go back to the hidden lens removed, what I want to use is what's called a breakout section. So come up here to view layout, and click over here under breakout section. Now breakout section just allows me to draw some shape, and then I can choose to remove that material down to a certain level.
So in this case here, I'm going to draw a little roundish shape here, and then I'm going to choose the depth. Now you can either type in the depth here, or you can choose something from a different view layout. In this case here, I'm going to choose one of these circles. There it is, it's going to choose the edge and it's going to cut the material out to that level, click on OK and you can see it remove that material down to that layer and you can see exactly what's going on with these holes intercepting with the other thru hole. Then you can come in here, use your regular annotation tools like the smart dimension and if you want to you can dimension you know, the angle if you needed to you can dimension the size of the hole.
You can add some notes as far as what's going to happen here when these two holes intersect. Maybe you have to add some special de-burring operation to make sure there's not a burn in that hole. All this information can be added at this point in time, because we're seeing what's really going on behind the scenes inside of this part by adding that breakout section. So that's a great way to use that tool. Now up here, I also have another hole I need to call out, and it's on this face here. You can see it here, kind of on an angle. So what I'd like to do is actually add a auxillary view. To do that, let's go up to View Layout. Click on Auxilliary View, and then choose an edge.
In this one, I'm going to choose is this one right here. And notice it automatically snaps that view to my cursor, and it's going to look like it's going to overlap this other part, so just drop it anywhere there. And then I want to move this so it's not overlapping my other part. So go ahead. And, right click on it. And come over here to alignment and say, Break Alignment. That will allow me to move this now down to my drawing sheet a little bit. I can move things over a little bit to get a little more space. And then, I can move the little a, indicating that view, and make it so I'm looking directly down on that face, and you can see over here, view a, showing that.
Now I can add some dimensions. Alright, so I can add annotation. And dimension move from this edge here to that hole, defining what it is, and coming up, and use a hole callout, and define that hole a little bit better right there, and now I can see all those different views, I can see all those different holes, and how they're being laid out on the sheet, and what's going on here, especially when you have holes that are intersecting. So a bunch of great tools within the SolidWorks toolbar to use and call out holes. And specify exactly what's going on behind the scenes.
As with many things in SolidWorks, there's a handy tool to call out holes. The tool does most of the work. However, make sure to double check the hole call out to make sure it makes sense. After all, we're just writing our inputs from the part file. So if we put the wrong value in the part file, keep in mind, it's going to be bringing in the wrong value into the drawing.
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