Creating Bracket Part Files in SOLIDWORKS Using Body Keep and Feature Isolation Techniques

In this lesson, we're going to create all the individual parts that make up the brackets of our playground. Before we get started, I just wanted to show you that I've placed not just the master file, but every single one of the part files we made in the last video, all in the same folder, both for organization and also it makes it easier for SOLIDWORKS to recognize part references from one to each other if they are all in the same folder. It makes it easier for SOLIDWORKS to find those parts.

So the first thing we want to do is open up our master file playground. Beautiful. Now that we've done that, we can identify there's a couple brackets that we need to create individual part files for.

I think we have one, two, three, and four. So let's go ahead and do that now. Go to File, New, make sure Part is selected, and select OK.

Just like before,  it places us in a sketch automatically. Let's make sure we close out. All right, and then we'll go to Insert, Part, select the master file playground since it is already open.

It recognizes it right there. It wants to place arbitrarily in space. We don't want to do that, so we'll just go to the green check mark and place it right where it was created.

And now we need to delete all the bodies except for the one we want to keep for this particular file. We'll go to Delete Keep Body, make sure Keep Bodies is checked. In this case,  for Bodies to Keep, let's move to this flat linear bracket right here at the bottom.

Close it out with a green check mark. Let's do a Save As, and again, my hotkeys are CTRL-Shift-S. I recommend creating a hotkey set for yourself as well.

Save As is something we do a lot. And for this, we'll call it bracket underscore 001. We're going to follow the same naming methodology.

Now, this is an incomplete bracket. There are no holes. I explained in the last video that there are some features that are unique to parts that I like to save for their individual part file as opposed to including them as features in the master file.

One, to keep the master file nice and clean with only the main design features, and two, if there's something that just affects a unique part, I want to leave it in its own part file so as not to mix it up with anything else. First, I'm giving these corners fillets of an eighth of an inch, 0.125. We're going to close that out. Next, I'm going to start a sketch on the main face.

Use a center line to connect the midpoints of all four sides. This is because I'm going to use the mirror feature. And then, let's grab the center circle tool and create a hole pattern for ourselves.

These holes are going to be a half inch in diameter. It's recognizing half an inch. Perfect.

I can place it exactly on this bracket, but I want to create the whole pattern first. So,  I'm going to go to Linear Sketch Pattern, select this as my entity to pattern,  and we'll give it maybe three instances. Give them a little bit of space between each other,  and just close it out with a green check mark.

Let's set a distance between this first circle center and the edge, and we'll set that as one. Better yet, let's set it as two. Now, let's determine where this ends.

Well, I want it to mirror, and I want the holes on the right to be equidistant to each other, just as the holes on the left are. So, the first thing I'm going to do actually is go to Mirror Entities, go to Mirror About, and select the three circles. And I don't want these too close to each other or too far apart.

I want equal distance between every single set of holes. So, to do that, let's go to Midpoint Line, start it on the exact center of our bracket, set it to a construction geometry,  use a center line to connect the edges of that midpoint line with vertical lines to either one of these circles here. Let's go ahead and start another midpoint line or center line right there from that circle and connect it there.

Then, let's go ahead and make this midpoint line and this regular center line equal to each other, and it should set our entire pattern. Once we've done that, we'll do an extruded cut. We can just go ahead and do it through all both.

There's only one item here, so that's okay. And we can go ahead and save it. Let's do the next bracket now.

We'll first do a Save As, set this name to Bracket002, delete the features unique to this particular bracket and the sketches as well. Before we continue, let's just go ahead and make sure we aren't importing unabsorbed sketches by accident. Oh, it's just doing solid bodies.

Great. If yours has unabsorbed sketches, uncheck it and go back to the other bracket and uncheck it in that one as well. Again, we want to keep our files nice and low on the burden that it places on our machines.

Let's edit this Body Keep feature, and let's find the next bracket we're going to use. In this case, why don't we use this angle bracket right here. All right.

Now, for this, we'll do two holes on this side and two holes on this side. So first, I'm going to start a fillet, and lucky for us, it remembers the last fillet we used,  0.125. Let's do that again. This is another advantage of using the same open part and just renaming it over and over because we get to keep the information from the features of the previous part we made.

Saves us just a little bit of time. Just like before, pick a side that we're going to put holes on and draw lines going all the way to the top. All right.

Now, let's grab a center circle,  set it here. We'll set the diameter of that center circle at half an inch. Let's mirror it along this line.

Okay. Now, I want these circles to be equidistant to each other as they are from their respective edge. So just like before,  let's use center lines to create that condition.

Let's go ahead and follow along. All right. Perfect.

Highlight these two, make them equal. They seem a little bit close to each other. Let's go ahead and undo that and maybe just set a distance.

In this case, we'll call it two inches. Great. That looks good.

We'll use our features to do an extruded cut,  and we can go ahead and do through all both. Let's do the same thing on this side. Although I have a suspicion we can probably mirror this feature over here.

Let's give that a shot. Let's go to reference geometry, select plane, highlight this plane, and highlight this plane at a 90 degree angle to it, and it's creating a mid plane between these two surfaces. Now, let's see if we can use this plane as a mirror surface of this particular feature.

Let's go to mirror. For face plane, select this new plane we created, and instead of doing bodies to mirror, since we only have the one body, let's do features to mirror. Make sure that box is highlighted, and then go to extruded cut.

All right. Perfect. Save us a little bit of time.

Let's go and save that work. Let's rename the file to the next bracket, which is bracket 003. All right.

Delete all the features unique to this bracket and also the sketches. Go to body, keep, delete. Delete what exists there in that box and grab this new T bracket here.

Beautiful. Just like before, let's use the fillet feature to round out these edges. Make sure you're selecting just the corners and not any faces.

Grab that, grab that, grab that, and see if we can locate that. Perfect. 0.125. That's what we want.

Lovely. Go ahead and save your work. Let's start a sketch on one of the faces, and as always, create lines to identify the exact centers of each of these arms.

All right. Let's do three holes here, three holes here, and three holes here,  all equidistant from each other. All right.

Let's start with one circle,  set it to our regular diameter of half an inch. Let's create a pattern, selecting that circle as the entity. Use one inch as the distance for right now, and why don't we do four instances.

Perfect. Next, let's set a distance between this circle and the edge,  and let's go ahead and make that one inch. Now we can go ahead and grow this out so it looks appropriate.

Let's go to mirror entities and select all four circles in this pattern. We're going to mirror about this center line here, and just like we did a couple brackets ago, we want to make sure that these two circles in the middle are the same distance from each other as every other circle is from every other circle, essentially. We'll grab a center line,  actually better yet, yeah, let's grab a center line, start one right here,  and then we'll grab a midpoint line, make that construction,  establish a vertical relationship between the ends of that midpoint line and the centers of these inside circles, grab another center line, connect it to that circle, highlight that line,  highlight the midpoint line, make them equal.

Perfect. Now we just need to add the holes in this bottom portion of our T. So let's go ahead and grab the circle tool,  and for this, we can just make it equal to our original circle so it has the same diameter. We'll set a pattern, but not in direction one, so we'll set that instance to one.

We want this going up and down, so we'll set it in direction two, and for entities to pattern,  we'll select the circle, space it out by an inch so we can remove the cluster that is created automatically, set it to four instances, and close it out. We have this one inch away from its edge, let's do the same thing down here. Perfect.

And then maybe for this, we make this circle the same distance from this edge as this circle is from this edge. So as always, we can use center lines to help create that type of relationship. You can see SOLIDWORKS is automatically snapping coincident and collinear relationships, that's convenient in this case.

All right, there we go. You should have something that looks more or less like this. Let's go ahead and extrude a cut through this entire piece.

We'll do through all both, that's perfectly fine. Once you've done that, let's save it. Okay, let's do one more bracket.

First, we'll do a save as and set this to bracket 004 as the name. Just like before, delete any feature that's unique to this particular piece,  including the sketches, and change the body and the delete body feature to our new bracket,  close it out, save it. Now let's make changes to this bracket.

We'll start by filling in the corners. You may have to use your scroll wheel to zoom in to capture those accurately. Set it to 0.125. Start a sketch on one of these main faces.

Use a center line to locate the exact middle of each of these arms. That's where our holes are going to live. Now let's go ahead and create a center line that goes from this corner to right there.

I'll show you why in just a second. I'm going to make sure that this line is equal to its mirror, and it is. Great.

All right, we'll grab a center circle. There we go. Set it on that line.

Give it a distance from the edge of one inch. Let's see. I think for this, we can use a pattern of four instances.

We'll select the entities pattern as the circle. Left to right is the direction we want,  so let's go ahead and stick with the X-axis in this case. Set the number of instances to four,  and set a distance of, say, one inch for right now.

We'll close that out. Now how do we want this to be oriented? Let's place it so the circle is right above this edge. We'll create a coincident relationship between this line and the center of this circle.

Perfect. Now instead of doing this again, this bracket is a perfect 45 degree or a perfect 90 degree with both sides being the same length, so let's go ahead and just use this line to mirror those entities. There we go.

We'll go to mirror entities, and we'll mirror about this line here. Select these four circles. Perfect.

Once we've done that, we'll go to extruded cut, through all, both,  close out the green check mark, and save our work. That's it for this video. In the next video,  we're going to begin creating sub-assemblies from some of these parts that we've been creating.