Practical 3D Scanning: Mesh Section Sketches
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Mesh Section Sketches
05.27
| 00:00 | In the extracting entities module we looked at how we can create a profile from a cross section of a mesh body using our Peel.3D scanning and reverse engineering software, Peel.CAD. |
| 00:10 | A very similar operation is possible in Fusion using mesh section sketches , but with some extra functionality that can be very useful for our application. |
| 00:20 | So, we're going to carry on with our turbo manifold that we transferred from Peel.CAD in the earlier transfer to CAD module to make use of this. |
| 00:29 | It's important to remember that this model is aligned with the origin, so the default planes align with the flange, with this plane aligned with the back plane, and these two aligned with the centre point. |
| 00:44 | Before we get started I'm just going to group all of these features in the timeline so everything we create moving forward will be shown more clearly. |
| 00:54 | So, we're going to jump over to our mesh toolbar and we're going to create a mesh section sketch. |
| 01:00 | The first step is just selecting the mesh body. |
| 01:03 | And then we can select the section plane. |
| 01:05 | In this case we just want to click that plane in line with the flange surface. |
| 01:12 | Now, we're just going to offset the section plane and drag that into the mesh slightly so it doesn't just sit on the surface and that's going to give us a nice clear profile showing all the features of the flange. |
| 01:26 | We can also use this X distance here to just modify that distance with a bit more control. |
| 01:32 | So, after clicking OK we'll see that there will be two features in our timeline. |
| 01:38 | So, the first one of these is a sketch and then the next one is the actual mesh section feature itself. |
| 01:45 | We're going to right click on the sketch and click edit. |
| 01:50 | Now, it can help here if we just hide the construction planes in the origin and we'll also hide the other sketches and it can be helpful to hide the body as well. |
| 02:02 | So, the profile shown in this kind of burnt orange color is essentially the line where the plane intersects the mesh body. |
| 02:10 | And this is just like what we looked at earlier when we were extracting entities in our Peel.CAD software and we created a cross section profile. |
| 02:19 | So, if we select the line tool, notice how we can't actually snap to the profile even if we have the snap preference selected. |
| 02:27 | So, the trick here is under the create tab, choosing fit curves to mesh section. |
| 02:32 | And here we can fit all different curves types to the mesh section. |
| 02:36 | For example we're going to click circle and then we're going to fit a circle to the mounting holes. |
| 02:44 | If we move around we can fit a circle to each of these mounting holes and the software will automatically fit that in the correct diameter based on the section profile. |
| 02:57 | Then we can just hit OK there. |
| 02:59 | Now, we could just leave everything as it is, but it's actually better practice to use some constraints to make sure everything here is aligned and the diameters of the holes are correct. |
| 03:10 | So, what we're going to do is we're just going to select all of those to start with and hit equals. |
| 03:18 | We'll also make sure the centers are in alignment with each other using the horizontal constraint. |
| 03:33 | Then we can actually use our verniers here and we can measure the real part. |
| 03:38 | And we can just double check the dimensions of these holes. |
| 03:42 | They come in at 9.5 millimetres, so it's best practice in this case to set the diameter of these holes to 9.5. |
| 03:52 | We could also set the spacing of all the holes with dimensions as well, but we'll just take the easy way out and we'll click the fix constraint and then we can just select all the holes. |
| 04:03 | Following this we can continue the process of creating the sketch profile using straight lines, slots, arcs and more concentric circles as well as constraints and dimensions. |
| 04:14 | This is a bit of a time consuming, but very simple process so we'll speed up this section and the result is a fully defined and accurate sketch based on the scanned profile of the flange. |
| 04:29 | So, we could use the exact same process to pull a mesh section from the turbo flange or we could move forward and use the cross section that we pulled from that in our PLCAD when extracting entities as well. |
| 04:42 | While it's possible to pull more profiles out of the mesh that could be used to create the solid model, what we've covered highlights a function of these tools. |
| 04:51 | The runners will be modelled in the next module using the pipe centreline entities that we've already extracted, so let's recap the main points before moving on. |
| 05:00 | Just like extracting entities, we can create mesh section sketches, which essentially capture the profile where the plane intersects the mesh surface. |
| 05:10 | In Fusion this is just a matter of selecting the mesh body and the section plane. |
| 05:14 | Following this we can edit the sketch and fit curves to the profile, dimensioning the sketch features and using constraints all with the intention of creating a parametric model. |
