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Center Mark's got a nice reference to a hole or arc center location. SolidWorks has a tool for inserting these or we can even set up our template to auto insert the marks as we go. Center lines can also be helpful in drawing for indicating the alignment of various features. To get started let's go ahead up here and we've got this part which is 19.2-1 opened up, and I want to make a drawing for that part. Go up here to file, make drawing from part. I'm going to go ahead and choose the TT template. If you don't happen to have that template using the standard template will be just fine as well. Click on OK, and it automatically generates a couple different views of that part and it automatically adds all these different center marks to my part.
Now I can zoom out, I can move things around if I need to, and I can even rescale the drawing by clicking on Properties and changing the scale. Let's try one to one, see what happens. That looks pretty good, so you can see a little easier there. Okay, now you notice, I've got all of these center marks pre-added to my drawing. And, what if I didn't have those, so I want to point out how that was actually done. Up here under Options, if you come up here under Document Properties, go in to Detailing, you can see, or actually, I'm turning on auto-insert, so when I make holes, it automatically puts the center marks. You can also add dowel pins center lines balloon, meaning that you can add all these things on view creation.
In fact, you can make these changes to your drawing template and anytime that you make a new drawing they will automatically show up in the drawing. If you need to manually add center marks you can do that as well. For example, if you didn't have these marks, if you wanted to delete these, you can just click on each individual one and hit Delete. But that can take a long time to delete all those individual center marks. I want to point out that we're going to use what's called the view selection tools. Now, I have them down here already, but if you didn't have those, right-click, come down here to Selection Filter, if it's off, you just go back again.
Down to Selection Filter, and turn it on you'll notice it shows up down here at the bottom of the screen. What I want to filter out is the center marks, so I want to make sure I'm only filtering center marks, then I'm going to window over that entire part, select all those center marks and hit Delete on my keyboard to take em out. When you're done with that selection filter go ahead and turn it off. Now I'm going to go back to the regular design. I can come up here to the top by the center marks, and I can add a center mark to my part. I can change how that center mark looks. I can change the default radius. I can change the extension lines, make any other changes I want to it.
And then if I click on this little icon here above it, it'll actually propagate to all the other center marks, all the other holes in that series. When you're happy with that click on OK, and it looks pretty good. Now we got these holes over here. And a lot of times, what I like to do is use Sketch > Center Line to connect the dots. So I'm going to connect from the center of each one of these holes, showing that these are a pattern that all work together. I can also come back up here under Annotation, and go over to Center Mark again, and add manual center marks as well. Showing the center points of those parts.
So I'm using these center lines to kind of show these are all in line in a series, so when I come down later and add a dimension, the dimension to the bottom hole. And it shows that these two holes are in line and their part of this little team of holes and work together. Same thing over here, dimensioning from one to the next one, showing that those are all part of the same team, without having to come up and actually. Drag that dimension all the way up to the top part. So, a great way to use both center lines and center marks. I also want to point out, we also have this command here called center line. Generally you're going to be putting a center line on maybe a rotated part that's going to be the same both sides, but in this case here you would probably not be using the center line.
But I do want to point out how it would actually be used. And if you click on center line, you can choose a center line by just choosing the two edges. So I'm going to choose this edge over here, and this edge over here, and you'll notice that it automatically adds the center line to the center of the part. So any time you see two edges, you can add a line between those to identify the center of the part. Center points and center lines are great for showing feature locations, without the need for excessive dimensions. Use these tool to link together related features to make it easier to understand and to use drawings.
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