Rhino3d Video Tutorials Transcripts - To further support you as you learn and progress with Rhino we've transcribed each of our video tutorials.
Hi this is Phil from Simply Rhino and in this video, we’re going to take a look at how Rhino3d can be used in conjunction with a parametric solid modeller, in this case, SOLIDWORKS. The idea is to create the a-surfaces or styling surfaces in Rhino and the engineering detail in SOLIDWORKS. We’ll look at how we can make effective use of file referencing to allow us to make updates and changes to both the Rhino styling surfaces and the manufacturing details contained in SOLIDWORKS without having to do any time consuming remodelling.
Let’s take a look at some of the basics of the Rhino and SOLIDWORKS workflow. Theoretically it’s possible to round trip Rhino and SOLIDWORKS native files but as you can see here, this in practice is not straightforward. SOLIDWORKS 2016 will only read Rhino version 4 files and Rhino version 5 will only read SOLIDWORKS parts and assembly files up to the SOLIDWORKS 2015 format. Thankfully, in the real world however, this isn’t too much of an issue, as the workflow with both step and IJIS files works extremely well and in some cases, better than using native file formats.
Let’s look first at something very simple. In Rhino I’m going to create some basic geometry and then read this in to SOLIDWORKS. So here we have a rectangle that is 50 x 100mm and I’m going to extrude this to a height of 200mm. Then I’m going to save this down as a version 4 file, just call this ‘box’ and then we’re going to open SOLIDWORKS and read the file in to SOLIDWORKS. So I can open the file directly here, by going to file, and open and finding my Rhino file and this will bring the geometry in to SOLIDWORKS and then SOLIDWORKS will perform a check on the geometry and here if we have any faces that are corrupted or edges that don’t join together, we’ll have the opportunity to fix these. Obviously with this simple geometry there’s no problems with it.
Two things to mention that are fairly obvious. First of all, SOLIDWORKS along with other engineering software, uses the idea of Y being the vertical axis rather than Z being the vertical axis. So in real terms, your geometry is rotated about the real world origin through Z to Y. The other thing that is slightly disconcerting for Rhino users is that the 3-Dimensional view in SOLIDWORKS, by default, doesn’t have any perspective applied to it. We can turn on perspectives here in SOLIDWORKS and out geometry looks a little bit more familiar.
The component will come in as an imported reference here and I can change the name of this component should I wish and then for example I could add some features to this. So let’s add some fillets here. I’ll just fillet these long edges here and accept this, and then let’s put a smaller fillet around the base and let’s then for example, shell this out to a thickness of 4mm. Okay, so that’s our geometry. So what we have are parametric features on top of a Rhino reference. I’m going to save this file as ‘SOLIDWORKS part’ and now if I want to actually update the Rhino reference, I can right click on my relevant feature here and I can edit this directly in Rhino. This will open a new instance of Rhino and the relevant file.
Okay, so now we’re in Rhino, let’s make a very simple change to this piece of geometry. Let’s turn on the gumball, use our sub-object selection and just reduce the height of this box by 100mm and then save this back out again over the top of our existing file and then we can go back to SOLIDWORKS and I can right click on my reference and I can refresh and this will update the geometry.
Okay, you’ll see here that a feature here has failed because the reference that I used to create the shell in the first place has moved. So on more complex geometry, it’s a good idea to supress the SOLIDWORKS features that you’ve added when you change the reference and then add them one by one. Here, I can edit the feature and re-insert the face that I want to shell out from and my feature will rebuild again. So we have parametric features on top of a Rhino reference that we are able to change.
Let’s now have a look at moving some geometry via a neutral file format. Here I’ve got a simple box that’s made from planer surfaces with the addition of some constant radius, tangent continuous fillets. There’s a number of steps that it’s worth going through before exporting the geometry to SOLIDWORKS and it’s a good idea to use solids in to SOLIDWORKS. So first of all we need to check that our geometry is watertight and I can do this by using the show edges command. This is found in analyse, edge tools and show edges. Just grab the geometry here and enter, and this will open the edge analysis dialogue. Here I just have naked edges selected with a nice bright colour here and you can see that essentially what’s happening here is that the top face that essentially joins the inner and outer wall of my box here is currently detached. So what I need to do is just join this all together in to a solid. This reports back that it’s a closed polysurface. I can check the edges again but if Rhino reports it’s a closed polysurface then there’s no need to do this.
A couple of other checks that it’s worth doing. First of all, I want to make sure that my geometry all passes check. So I can do this by either selecting bad objects here or by picking the geometry here and running the check command and then because my geometry contains trimmed surfaces here, I can run a command called shrink trimmed surfaces and what this does is that minimises the untrimmed area of the surfaces. So this command is in surface edit tools and it’s called shrink trimmed surface and I can select the whole polysurface in one go here.
Next, to keep the geometry in the same relative orientation once we’ve moved it in to SOLIDWORKS, I need to rotate about the world X axis, through 90 degrees. So I can do this by going in to my right viewport here, picking the geometry and going to transform and rotate, typing in zero for the centre of rotation and then rotating through 90 degrees so my Z effectively becomes the Y axis in world terms.
Okay now we’re ready to export the geometry to SOLIDWORKS so, what I’m going to use here is a step file and give this a name, and I’m going to pick the third of the options here which is AB214 Automotive Design CC2. The options here progressively give me more information in the step file. Okay so now I can go in to SOLIDWORKS and I can open the file, so it’s Tray SDP and you’ll see that the part comes in to SOLIDWORKS. Once again, we have the import diagnostics dialogue box which we’ll say yes to and our geometry passes check here. There’s nothing that needs fixing on it so I’ll okay that.
Now one of the things that we can do here, where we have fairly basic geometry and by basic I’m really talking about geometry that has rolling ball, constant radius fillets, planer surfaces and fairly regular features. If this is the case, we can proceed with feature recognition in SOLIDWORKS and what this does is that it attempts to create parametric features from some of our Rhino surfaces and if I just okay the automatic mode on this, then what should happen here is that SOLIDWORKS will create a plane and then it will create some features relative to that. And so now our original imported piece of geometry is no longer there and we now have a number of SOLIDWORKS features. Now sometimes, these features may not exactly equate to how we built an object but in this case for example, if we look at the fillets here on the outside, these features are in a way parametric so we can change dimensions on here. So let’s reduce this radius here from 20 to 15 for example. Okay, and you’ll see those radii change there.
Now one of the things that you’ll see here is because this object has had features added to it in a reverse sort of way, there is not a connection between the inner and outer fillets here. So we need to find those inner fillets and also edit that feature too and reduce that feature also by 5mm.
So it’s not a complete solution but it does have the ability to parametrises some basic Rhino geometry. However, for the most part, the real value of using Rhino is in actually bringing in geometry that would be very difficult to create in SOLIDWORKS. So generally speaking, we wouldn’t want to use the feature recognition tool. Now let’s take a quick look at exporting via IGIS.
So once again, I’ve got a couple of solid pieces of geometry here. I’m going to rotate these about the world X axis, through 90 degrees Z to Y and then take this geometry out via an IGIS. So export selected, pick IGIS and give this a name. And I’m going to use the SOLIDWORKS solids file type here and then let’s open SOLIDWORKS and open the IGIS file. Okay, and again we’re prompted for import diagnostics and we’ll say no to the feature recognition.
What you’ll see here and this happens with any file type, is that if you have for example two solid bodies in the Rhino file and you opt not to use any feature recognition, then you’ll have two separate references here and this is actually useful in certain circumstances and we’ll look at this when we look at the engine cover model. You’ll also see with the IGIS files, that the IGIS files maintain the object colour that was applied to them inside of Rhino, and as the default object colour is black, then it can make these objects a little hard to read in SOLIDWORKS. So to change this, we just need to go to our display manager tab here and then we can just remove the appearances that actually came in with Rhino and get these back to the default SOLIDWORKS appearance.
Now let’s look at bringing in some more complex real world geometry in to SOLIDWORKS. This is the engine cover shown at the start of the video and this is built from considered slab surfaces that whilst all being double curvature have been optimised to ensure a relatively good surface quality. The transitional surfaces are all G2 curvature continuous blends and creating an object like this is really the preserve of software like Rhino. Whilst we could shell out the moulding and add features such as holes and edge fillets in Rhino, the benefit of doing this in SOLIDWORKS is that of course these features remain parametric. So moving holes or changing the shell thickness should be relatively straight forward. This geometry is watertight, check and all the trimmed surfaces have been shrunk.
It’s a good idea to work on a copy of the file to export or as in this case, to copy the geometry on to a new layer before exporting. With exporting, the general rule is that step works well for simpler objects but that IGIS is better for more complex entities. So in this case, let’s use IGIS. So I now have the engine cover in its correct orientation ready to go in to SOLIDWORKS but before I export this, I’m going to create a small piece of secondary geometry here and this is going to come in as a second referenced object in our SOLIDWORKS model and the idea of this is that this gives us the opportunity to bring in a second object later on in to the SOLIDWORKS file if we need to do so. An example of why we might need to do this would be if we had a piece of geometry that was difficult to create in SOLIDWORKS and we needed it as a reference for a feature that was going to be created in SOLIDWORKS. We could create this in Rhino and export this out and replace the reference of this cube with our new piece of geometry.
So I’m going to take both pieces of geometry now and export them out as an IGIS file and I’ll call this ‘engine cover’. Let’s call it ‘engine cover 01’ and we’ll use SOLIDWORKS solids again and then we’ll open our SOLIDWORKS and open up this file. So our geometry comes in and we’ll be prompted to run import diagnostics and we don’t have any issue with either of the two parts here. We don’t want to proceed with feature recognition, we want to keep these two as references. In the case of this object, our bonnet here, then feature recognition would really fail to do anything here because we have got an object which is built entirely from complex surface.
The first thing I need to do probably is go in to my appearance manager and just remove the black appearance that’s come in from Rhino and then just change the display style here to make this a little easier. Then I’m going to name my imported feature here. So this is the ‘engine cover’ and this here is my ‘spare part’. So not really interested in that spare part at the moment, so I can supress that feature here but it remains in the tree but it is just hidden. So now I can add some features to this geometry.
So we’re going to start off by adding a shell to this and the shell command does something very similar to the Rhino shell command. So I’m going to give this a thickness and then just as in Rhino, I nominate the faces that I want to remove as part of the shell process. Now this area here has been modelled, particularly so that we can replicate what would be a kind of sensible C and C trim in the case of this GRP moulding. So we remove the base and also the back face as well. When we’ve picked all those faces that we want to remove, I’ll enter this and create the shell.
Now typically, in SOLIDWORKS, a command will either work or fail rather than in Rhino, where the command will fail but give you the parts of the geometry that it can make. But just because the command has actually worked in SOLIDWORKS, doesn’t necessarily mean that all the surfaces that are created, for example by the shell command are going to be perfect and to that end it’s worth just having a look at the underside of the shell here and checking the layout of all of these constituent parts.
Typically features like fillet which resolve to a point would be difficult to offset and again very similar to Rhino, features for example, a small fillet that shelled inwards where the original radius was less than the thickness of the shell would potentially cause problems in SOLIDWORKS as well. So it’s worth just checking that geometry out. Then we can go on to add some further features. So I’m going to add some fillets now and we only need to add some small fillets here, really to help the moulder out. We want to avoid sharp edges wherever possible on this, or seen sharp edges so that we don’t have any parts of the moulding that are breaking off when it’s released from the tool.
So I’m going to put a 6mm fillet here on the short corners of the features. So just so I don’t pick the wrong edge here I’m going to disable tangent propagation and I’m just going to pick the six areas here. So you can see that I’m something of a novice user in SOLIDWORKS here but should at least show you the workflow between the two pieces of software.
Okay, so those are our corners done and then I’m just going to look at doing the outside edge. So again, another fillet here. Let’s give this a 2mm radius, turn on the tangent propagation this time and pick this outer edge and all that edge should highlight and run a 2mm fillet all the way round the edge.
Okay, next up I want to go to my top view and zoom in to this area. This is where we’re going to put a hinge to open the engine cover and we want to put some holes in here to accept the hinge. So I’m going to add a sketch here and I’m going to make that sketch relative to the top plane and I’m going to then choose a centre rectangle. So to add the hole detail, first of all I need to create a sketch in SOLIDWORKS and I’ll create a centre rectangle and I need to make this relative to a plane so I use my top plane here and I need to make this a sketch with some numeric input. I’ll find the centre of this plane here and drag outwards and I’ll make this 60mm in the one direction and 100mm in the other dimension and okay that. Then I can exit the sketch and then create the holes as a feature. Make these holes 12mm, position them on this face and add the holes and accept that and then let’s switch back to a 3-Dimensional view and let’s mirror that whole feature to put it on to the other side. So we’ll mirror, and we need to pick a plane about which we want to mirror, so that will be the right plane and then the feature that we want to mirror here is going to be the hole and we’ll accept that.
So you can see now that we can add a number of parametric features in to our model now. So we have a Rhino reference and plenty of parametric features added to that. Now in the real world, what we might have is a more complex part than this and let’s say between 50 to 80 parametric features that are added in to our SOLIDWORKS model and there are times where your customer or your co-worker or your client may request a modification to the geometry that can only be done in Rhino.
So let’s say that we were required to put some scoops in to this bonnet which needed to be curvature continuous and controlled very tightly with the existing geometry. Clearly this is something that we’d struggle to do in SOLIDWORKS and yet we’ve done all this work in terms of adding features and we don’t want to lose that work. So this is where we can actually, using a careful workflow, where we can actually update the reference and re-propagate our features.
So first of all, I’m going to save the file and save this as ‘engine cover 01’ and then I’m going to go back to Rhino. So here’s the same part in Rhino and let’s jump to the modification that we need to make to this. So what we’ve done now is added the scoop and mirrored this over to the other side. So again, in Rhino this is a curvature continuous feature and this again is something that would be best done in Rhino rather than doing it in SOLIDWORKS.
An additional complication here, is that also in the scoop we want to add a particular cut out to this and of course, the shell is actually being done in SOLIDWORKS but we want to actually be able to reference the shape for the cut out inside of Rhino and let’s say the part that we want to produce our cut out with looks like this. Because we’ve got this spare reference in the file, this actually gives us a way out of doing this. So if we look at the same parts in their orientation ready to go in to SOLIDWORKS, what we can do is to save this out as two separate IGIS files. So we’ll take this file here and export it out and we’ll call this one ‘engine cover 02’. And we’ll take the part that we’re going to use as our Boolean cutter and we’ll export this out as ‘cutter’. Okay, and now we can go back to SOLIDWORKS.
So inside of SOLIDWORKS now, the best workflow here to do a save as, to preserve our original file and we’ll save this as ‘engine cover 02’. Now when we’re bringing in complex geometry, there’s a chance that some of these subsequent features may not work. So to avoid having some sort of calamity in SOLIDWORKS, what we can do is we can essentially pick all of the features that we’ve added and right click on them and supress them. So we get back down to our starting Rhino geometry and I’m going to unsurpress the ‘spare part’ reference in here. And first of all I’m going to change my reference for the engine cover. So right click on the engine cover reference here and click on edit feature. This will propagate a warning telling me this is a reference file and I accept that warning and I replace my geometry which was ‘engine cover 1’ IGIS file with ‘engine cover 2’ IGIS file. And the Rhino geometry will now come in and my reference will be replaced and you see I’ve got my new part here. Then my spare part, I can also edit that feature and replace that with the ‘cutter’ and that cutter comes through in position.
Let’s just go to the display manager and remove the black appearance and change the display style. It’s important to understand that although the definition of the vertical axis is different in Rhino and SOLIDWORKS, the absolute position of the parts in 3D space is the same. So that if the relationship between the cutter and the bonnet was correct, then it will be correct in SOLIDWORKS. There is one caveat to this, is that if you are working on a file and bringing in new parts, or new references then be careful about working in perspective mode, because we’ve seen in some circumstances that perspective mode has troubled SOLIDWORKS idea of absolute, 3-Dimensional space. In other words, what’s happened is that we’ve had perspective on, brought in an object and it’s come in at the wrong position. So as long as we’re working the default parallel projection we should be okay with bringing in geometry like this.
I’m going to change the name of this part now to ‘cutter’ and for the moment I can supress that cutter because I’m not going to use it at the moment.
Now what I can do now one by one, is to unsurpress these features. Okay, we should find that all of these will work but it’s a good methodology to turn on these features one by one. So I have the holes back, and then the mirror back. You should see that all of these files add correctly. So now we have our new shape brought in to SOLIDWORKS and we can then turn on the… or unsurpress the cutter and we can either use this as a reference in SOLIDWORKS to create a sketch and to do a cutting operation with that, or we can actually use this geometry to… as a Boolean process. So let’s do the latter to make sure that we’re actually using the Rhino geometry here rather than a repurposed version of it.
So first of all let’s run the mirror command and we want to mirror a body not a feature and for the mirror plane, we want to use the right plane and for the body to mirror, we want to pick our cutter. So our cutter now exists in its opposite hand version. Then we can insert a feature called a combine and we can select the main body here and the subtracted features here, making sure that we’ve got subtract selected here and we can produce our cut. So now we have a component that has a whole set of parametric features and whose shape we can reference and update by changing the original Rhino file.
So in the real world, this gives us a pretty flexible situation where the basic shape can be updated inside of Rhino and the parametric features can be updated inside of SOLIDWORKS and the sets of features will co-exist quite happily.
I hope you’ve enjoyed this video, please look out for further videos from the team at Simply Rhino.