Transcription
In this tutorial, you will learn to make the base plate with borders for the Gridfinity system. This will be fully parametric and will allow you to control the number of rows and columns, the individual sizes of each border, the magnet diameter and depth, and the top offset. The in-depth version of this tutorial is also available for our members. Welcome to the Learn It Channel. Let's make the ultimate Gridfinity base plate design.
So, the first thing we're going to do is go to our parameters. And here you can find it under the Modify drop-down menu, Change Parameters. And if you click on the kebab menu, you can pin it to the toolbar or shortcuts. So, let's click on Change Parameters. And the first one we're going to put in is the size of our base plate design or the square size of the individual pockets. Now, I'm going to put a link in the description below to the Gridfinity Design Reference, and I hope you open that up and follow along with me. So, here we're going to call this our square dimension, and we're going to specify this as millimeters, and we're going to call it 42 mm. And let's just go OK. And because the rest of our design is in millimeters, let's go up to Document Settings and change the active unit to millimeters. Now, that's all we need to create to start.
So, the next thing we're going to do is create a sketch, and let's create it on the XY plane. If you're struggling to see the canvas just like this, make sure to go to your Preferences. Click on that and then Default Modeling Orientation, select Z Up, which is the standard direction for most 3D printers. So, select Z Up. Let's go Cancel and create a sketch on that XY plane. Next, create a two-point rectangle. We're going to place it at the origin. And here, we're just going to start typing in our parameter, square dimension. Tab to go to the next one, square dimension. Enter.
Now, we're not done with this. Let's just bring our part down here. And we're going to go back to Change Parameters and let's put in some parameters for our columns and rows. So, let's just type this in, columns. And for our unit, make sure to select no units. And let's just put in two columns for now. And we'll do the same thing for rows. Let's go OK. And remember with an Excel spreadsheet or standard spreadsheets, columns go up and down and rows go left and right. So if we go to this parameter right here, let's go square dimension times, and we'll type in rows and enter. And then over here, we're going to do the same thing, times columns. And we use the asterisk or Shift 8 for the multiplication symbol.
Now let's just test our parameters. I always encourage my students to test often. So go to your parameters and let's just change our columns to one, which is looking great, columns to three, rows to five, rows to two. It all is looking really good right now. And I'm just going to set it back to two and two. Let's go OK. And we can finish that sketch and go to our ISO view.
Now let's press E to extrude. You can also go up there, but E is the shortcut. We're going to go in the up direction. So grab your arrow and here it's a positive value. So at this point, let's look at our design reference image on the Gridfinity website. And here you can see that the enlarged base plate, it's the bottom right image. We're going to input all that information. So here we go, 2.15 mm + 1.8 + 7. Now this is going to be the thickness of our Gridfinity base plate.
Now, at this point, let's put in our margins or our borders. And if you think one word is better than the other, then please type it in the comment section below. Would you use borders or margins? Anyways, let's go to parameters and we're going to add another one. And I'm going to use borders in this tutorial, but again, let me know what word you would prefer. So, here I'm going to type in border front, border back, border left, and border right. And for each of these, I'll just specify 10 mm as the expression. Now, make sure to either put an underscore in between your words or just space them with capitals. And right now, this is actually called the Pascal case form of typing in our parameters. So, let's include the rest.
Once we have those in, we can just go to our Modify drop-down menu and press pull or Q. And here we're going to add a press pull to each of our faces and add the parameter right there. So just type in front, and that's going to be our border front. And right-click to go to the last tool, repeat, press pull. We're just going to go to the back there and type in border back. And then do left and right as well. Perfect.
Now let's just make our origin visible. And we can prove that our parameters are working well. So our border front, let's just go down to zero. And then you can see there it's perfectly aligned with our origin. The left as well, let's go to zero. And that's perfectly aligned with our origin as well, the YZ plane. And we can do the same thing with the back and the right just to test everything. Let's go to 10 mm. Again, I'm just going to add that for the sake of this tutorial. And then we can change it. And I like to encourage my students to test their parameters often again. So, let's go there and there, and there we have a beautiful base plate so far. Let's go OK.
Now, here we're going to create a sketch. And we need to create two sketches actually. The first is going to be the perimeter of our pocket. And so, here I'm going to just going to create it on this top face right there. And I would like to use this origin point. So, that's the benefit of creating everything around our origin or at least the main size of our base. But we can use our two-point rectangle and grab that right at that origin point and type in square tab square. And there we have it. So this is now locked to the origin. And if it isn't, you can always constrain it, coincident corner to the origin right there.
Now the next thing we're going to do is we'd like to actually create this as one single path for our sweep tool to follow next. And at this point, we need to put the fillets on each of the corners. Now, you might be saying, "Learn It Channel, I've heard elsewhere that we should never put fillets on our sketches." While I agree with that most of the time, this is an instance that we should use the fillet tool to create one single path for our sweep tool. So, I'm going to do that right here.
Now, if you'd like to go into the nitty-gritty of all of this, I've actually created a behind-the-scenes tutorial for all of our paid Patreon members. And so if you'd like to see the reasons why, I encourage you to click on the link in the description below to take you over to our Patreon site where you can learn not only about this and problem-solving regarding this, but also so many other tutorials that I think you would find incredibly beneficial. So once we've selected our fillet, I'm just going to go and click on the corners and add a fillet to each of these. And you see we get a little alarm down here, constraints and/or dimensions were removed. Don't worry, we're going to test that this actually works. But here, we're going to put in our radius value on the Gridfinity Design Reference. We can see that they used 8 mm. This is the diameter, but our fillet value is entered in radius. So, type in 4 mm as our fillet value. So, here we have it. Everything is constrained. If we expand our sketches folder, you can see sketch 2 is fully constrained. So, this looks great. It's one single path. And we can double-click that to select the entire path. Everything is looking great. Let's go finish sketch.
And now here what we're going to do is we're going to create an offset plane. Grab our XZ plane and move this on over to the exact center position of our profile. And so this is square divided by two. Now let's create a sketch. And we can actually right-click that plane and go create sketch to create a sketch right there. Now, we'd like to utilize this geometry that we just created. The best way that we can do that is by pressing P. P for project. Make sure specified entities is selected. And I'm just going to pick these two outside edges right there. And go OK. And what that does is it projects it onto the current plane that we are sketching on. If we hide our body, you can see that we've got this nice line that we can work with right here. And this is actually sketch number two. But if we hide it, we've got these two endpoints, which is exactly what we want to work on.
I'm going to create a two-point square and grab the origin and then grab this top point right there. Next, I want to put a reference line down the center right here. And this is going to be our center line. Now, just to show you a little tip, I could search with my mouse and try and find that triangle, which is the center point. Or I can just create a line off into space over here and then click the midpoint constraint, endpoint to line, and that automatically locks it. Endpoint to line. So that locks it in.
Now I'm going to move on over here and sketch the profile for our enlarged base plate. So here we have it. We're going to go on an angle. As we move this on the same angle, you can see those lines are automatically constrained. If they're not, that's okay. We'll just go up to the parallel constraint and specify those two lines as being parallel. Now D for dimension. Grab those two lines right there. This is going to be 45 degrees. This goes a little bit crazy. That's fine. Just drag it. There we have it. D for dimension. Grab our line. And right there, that endpoint. And this is going to be 7. The next line is going to be 1.8. And this one is actually fully constrained, but we can still call it a reference dimension. Create driven. And now it says 2.15.
Now we've got this beautiful profile over here. If we go escape, it turns blue. This means that it's closed. We can go finish sketch. And now this is what that sketch 2, this entire profile is going to help us with. So if we go create and we go to sweep, we want to pick this profile and we want to sweep around this path. Now we get an alarm saying we can't see it. That's because bodies is hidden. If we make it visible, now we get this perfect profile that we can work with. Let's go OK. And let's just check to make sure that our parameters are working. Again, we can go down to one column if we want one row. Borders we can take right off. And this is not breaking for us. So this is looking great. I'm going to go back up to 10, 10, and two columns and two rows just so it makes more sense. It's easier to compute in our own mind if we do it this way and then adjust it later on. But make sure to test often. Let's go OK.
Next thing we're going to do, well, we can just hide our origin. I'm going to go to the extrude and I'm going to go down here and we're going to move this a certain distance along with our center position right there. But let's go cancel for a moment. And we're going to go back to parameters. And we're going to now create two more parameters. And this is going to be our magnet diameter. And let's call this 6 mm and our magnet depth. And we're going to call this 2 mm. So let's go OK.
And now we need to create a sketch on the bottom. Creating a sketch on the bottom, it actually inherits the geometry for our cutout. If I go undo and just go to extrude, you can see that I can't actually pick the inside of that pocket right there. But if we right-click and oh, right-click on the face and then go create sketch. Now it creates another profile that we can extrude right here. So let's do that. E for extrude. And I'm going to pick both of those. Let's move it on down. And we're going to go magnet depth + 1. So this is always going to be 1 mm deeper than our magnet. So there we go.
Next, we're going to create a sketch on this face. Let's do that. Create sketch. And it inherits all this geometry as well. So we can work with that. For example, it will find the midpoint. Let's put a line from midpoint to midpoint and do the same thing over there. And in fact, I'm going to press X on these lines to turn them into construction lines. Next, our center diameter circle. We could do the math right here, but I would like to just put in our magnet diameter. And then the math, if we calculate it correctly in the design reference, all we need to do is pick the center point to our center line. And this is going to be 13 mm. And we'll do the same thing over here, 13 to 13, just like that. And in fact, I could get rid of this dimension and just click this one. And they're exactly the same.
Now, I'd like to save the fillets to the very end. We're going to do that when we're working with a solid model. But here, I'm just going to create these two lines to represent some sort of enclosure for this magnet. And here, we're going to press D for dimension, click the line, and then right-click, pick circle, arc tangent. And that's going to force it to pick this quadrant point of our magnet. And here we go. We're just going to specify 2 mm. Let's do the same thing down here. Right-click, circle, arc, tangent. Grab that quadrant. And we can move this on over as well. Let's click this dimension to make sure they're both 2 mm. And there we have it.
Now, let's mirror all of this. If I want to pick a chain, I'm just going to double-click. And they both those lines turn blue. I'm going to pick the circle as well. And the mirror line is going to be right there. Let's do the same thing. Right-click, repeat mirror. Double-click, single click. Double-click, single click. Mirror line is going to be right there. Let's go OK. We can finish a sketch now.
And now let's go extrude and grab this profile. That was one reason why we made these lines into construction lines because this is now one profile instead of four. So we can pick that distance to object. Let's pick the underside. Let's go OK. Let's bring back that sketch. And I'm going to go extrude and grab all of these circles for our magnets. And again, if I we're confused about which direction to go, just pull the arrow in the direction you want to go. And you can see it's a negative value. So let's go negative magnet depth. There we have it.
Now we can hide our sketch. And at this point, I'd like to encourage you to rename your sketches to keep everything well organized. So I'll do that. And there I've named them. And now I've just given them simple names in order to easily reference them later. Great. Now you can hide that if it's still visible. If it's still showing this closed profile, make sure to hide that sketch.
And now we can just go right into fillet. And I'm going to show you a little secret here. Go to your home view. And I'm not going to orbit at all. I can pick these edges. No problem because they're visible. And we can pick that one and this one. But with our cursor selection here, hover over selection filters and make sure select through is selected. And there we can actually look right through our part and we can grab those other edges. No problem, just like that. And I'm going to say that these are going to be 5 mm. And I think that looks pretty good. You can adjust that. Oh, and I missed one. So, let's go on over there. Just hold down Command on a Mac or Control on Windows and you can pick additional edges or deselect edges too if you'd like. But this is looking really good. Let's go OK.
Now, at this point, we can create a pattern and make sure to pick features. Features are basically any tool that we've created in our timeline. And here, we're going to pick this sweep. Skip over this extrude. This is the bottom face that we extruded. But I'm going to pick these other two extrudes and the fillet tool. And now our axes. We can either pick them on our origin or any axis of our part. I'm going to pick this edge. And that specifies our X-axis. Then I like to drag the arrows. Next, we're going to drag the arrow over and let's work with what we've got so far. I can adjust the dimension here or on our dialogue window. But instead of extent, I'm going to go spacing and then here again, we're going to specify this as the negative value, square dimension, and then the number of columns in this instance. There we go. Let's go Enter.
And I failed to do the other one. So, we're just going to double-click and go in the other axis. So, make sure to go to axes up here. And I can pick the Y. There we have it. Actually, we've created a little bit of a problem here, but this is easy. Let's go to axes. And we can hold down Command and pick the other edge. And that should work for both. If that doesn't work, no worries. Just go to our distance over here and type in something and our quantity. And that should work for us. No problem. OK.
So, spacing is selected. Distance is going to be square. And this is going to be our number of rows. And the other distance, just grab the arrow there. And we're going to type in square and columns. And it's going the wrong direction for some reason. So, make sure to go the opposite direction. If this ever happens, just go opposite, negative direction, negative direction, and that should solve it. So, now let's test everything. Let's go to parameters. We can go to columns of three, rows of three. Turn off our borders if we want. Let's go to the front border, zero. The back border, excellent. Left and right. And everything is looking really good.
Now, we're still not done. We've got a couple other things to do, but while I'm resetting that, I'd just like to send a shout out to our sponsor. Thank you so much, PCBWay, for sponsoring this tutorial. Currently PCBWay is having an 11th anniversary sale. So if you head on over to their website, you can see that there are certain deals, there's specials, there's all sorts of different things. I've been working with PCBWay for over a year now, which has been great. And I'd actually like to just highlight one project that we created. It's a project that we made on our channel. We designed it, but we had it manufactured with PCBWay. And they did an amazing job with brass. They made the safety razors. And since then, we've actually ordered five more assemblies of stainless steel razors and adjusted them just a little bit. Anyways, they do a great job. They're easy to work with. Their prices are very reasonable. And again, we'd like to thank you very much, PCBWay, for all of your support. Hope everyone that's viewing this goes to check them out. A link is found in the description below.
So, we're not quite done yet. Let's go back to our fillet command. And I'm just going to pick these four edges over here. And I'm going to specify the same dimension, 4 mm for the radius value. And of course, you can adjust this however you want. You can always go back to the fillets and you can make them bigger or smaller. You could actually make them as individual fillets by hitting the add selection set. And what that does is allow you to control other aspects and with a different distance or value. So, we're going to do that. Let's just go cancel. And we've got 4 mm on each of these, which is looking really good.
Now, one last thing that I want to adjust is I don't want to have this as a perfectly sharp point. This isn't going to do very well with our 3D printer. So, what I'm going to do is do an offset plane and then just pick the top surface. And I'm going to go down and let's go to 0.5 mm, something like that. In fact, I would like to create a parameter for this. I'm going to create a parameter called top offset and let's just go 5 mm. Let's go OK. Back to the construction plane. And then instead of minus 0.5, we're going to go minus top offset. There we have it.
So once we've done that, we can go to split body, pick our body to split, and our splitting tool is going to be our plane. We can go OK. And then here under bodies, you see we have body one. And when we click on that, that's the one we want to keep. Body two is the one we don't. So click on that and go remove. Don't go delete because it will break your model. If we go to construction, we can hide plane two. And now we've got this nice flat. And if this is a little bit too much, we could always go back to parameters and to our top offset. And we could make this a little smaller if we wanted. We could make it a little bit bigger. And you can see everything is updating right away because of our parameters. So let's go back to 0.5 mm. I think that looks pretty good.
Now let's conclude it with something that I think is going to be very useful because I would like to know the entire width of this without having to calculate it. And then I'd like to create another parameter that's going to help me to see how much more material I need to add to either of these borders in order to make it the desired shape or desired size that I'd like. Let's go OK.
Now, before the fillet, I'm going to go back in time before this fillet. And so that these edges are square. Let's go and create another sketch. I'll create it on the bottom over here. And I'm going to press D and just pick that top edge and create a driven dimension. Same thing over here. Create a driven dimension. Perfect. Let's go finish sketch. And we can also go to parameters and make sure that our number of columns is three. So we know that these are going to be different values for those two references that we've created. So let's go OK.
Now, for some reason, this is being shown again. So we can hide that sketch. No problem. And now what we can do is under our parameters, we can go back over here, expand our model parameters, and go all the way down to the sketch that we just created, sketch number six. And you can see we've got two bracketed dimensions. So let's star them. That turns it into a favorite. And now we can rename this. So I can just call this the total width. Enter. And this is the total depth or whatever you want to call it. So there we go. If we expand our columns, if we say that we want four columns, you can see that all of a sudden this is the total width right here. This is the current total width. And of course we can change the left border. And then this will update automatically. And our right border. Perfect.
So I'd like to create two other parameters right now called our desired width. And let's say I'm just going to specify 200 mm for now and a desired depth. And we say we want this as 150 mm. So that's looking really good. Now let's favorite those as well. And these will favorite and it will keep the order of our favorites until we actually click on these top headers over here which will change everything. But if we favorite them, it will save it in the order that we'd like. So here we've got our desired width, our total width, and so on.
Let's create two more parameters. And I'm going to say add border width. And here we're going to specify our desired width minus our total width. And you can see now it's saying that we've got 24 mm to work with. So we need to add 24 mm extra to our borders in order to create our total width. So we're going to do the same thing over here. Add border depth. And this is our desired depth minus our total depth. And we're going to favorite that as well. So now you can see, yeah, we've got an extra border we can add of 46 mm. But because our square is 42, we could actually say we want an additional row. And now we only need to add to the border 4 mm. So if we look at the front and the back, we've got 10 and 10. If I say 12 and 12, and look at our desired width is 200. Oh, of course, I've done the wrong one. Sorry about that. Our desired width is going to be 24. So let's add to our left and our right. This divided by two is going to be 16 mm there, 16 mm right there. Perfect. So our desired width is 200. Our desired depth. Our total width and depth is spot on. And we need to add 0 mm in order to compensate. So this is looking great. Let's go OK.
And then last but not least, we're going to drag our timeline to the very end. And our product is done. So, literally, we've just got a little bit more. We're going to finish this off very quickly, but if you've learned anything, make sure to thumbs up. If you love us, please consider subscribing or becoming a member and helping us out that way. And we'd love to hear from you too, how you've been able to utilize these tutorials to help you with better organization.
So, now let's test our model before we conclude. And we're just going to adjust the columns and the rows. Make sure that we test our border front as well. If we go to zero, that this doesn't break for us. Zero, zero, and zero. That's perfect. Magnet diameter, let's go to 5 mm. That all corresponds and updates automatically. Our magnet depth is going to go one. And you can see because we created a parameter, the bottom here corresponds to the magnet depth. So, if we use 4 mm magnets, there we have it. They'll never break through. And our top offset as well. Let's go to 1 mm. Yep, that's working perfectly. This part is done. Thanks for learning with the Learn It Channel. We'll see you at the next tutorial.