[LinkStage3] Tutorial, dome shaped geometry using loft in PartDesign.

[Music] hi to all how is it going so in the comment section under one of my videos i was asked how one can model this dome-shaped geometry and it turns out it is not all that difficult before we start i just wanted to let you know that for this tutorial i'm using release 10.15 of link stage 3 from real thunder and you can download it from here and if you like how the interface is set it up i made a video about it and you will find all the necessary links in the video description one thing to note is that this process should work just the same in link stage 3 as in master so let's start as usual we will go step by step trying to achieve the final geometry and in this particular case we can see that the geometry is controlled by these datum planes to be more precise the geometry dimensioning is controlled by the datum planes using sketches map on them we will start by creating a new file and if you followed my tutorial on the interface customization press w on your keyboard for the workbench switcher and switch to part design let's create a new body we will rename it as perhaps loft and we will create a sketch mapped on the x y plane press ok using the construction geometry we will create a 50 by 50 millimeters rectangle so shift h on your keyboard 50 millimeters select these two edges and make them equal by pressing e on the keyboard and we will make it symmetric by selecting these vertices here and press s on the keyboard toggle off the construction geometry create a new rectangle let's loosely draw it in here then using the fillet tools we will fill it all these edges here right click to dismiss the tool select the four arcs we just created will we will make them equal by pressing e on the keyboard and we will give them a radius of shift r 6 millimeters select these vertices here and the center of our sketch press s on the keyboard for a symmetry constraint we need to make this edge here and this edge here equal by pressing e on the keyboard then select this vertex and this line and we will make them tangent by pressing shift o on the keyboard and we have a fully constrained sketch let's just close it and get back at our example file as we've said the geometry is controlled by the positioning of these datum planes we will hide this 45 degrees datum at the moment to have a clearer view and we can see that the overall height is controlled by the positioning of the top datum plane and we can see its attachment offset in the property view under position and the z offset is 45 millimeters another important one is this screw level datum which controls the height of our dome base and again we can see the attachment offset position and the offset of 5 millimeters and this midplane here controls essentially the curvature of the whole geometry so let's start by setting up our datum planes and go ahead from there i will first create the screw level datum we will map it on the xy plane and we will give it an offset in the z direction of 5 millimeters click ok let's rename it as screw level datum let's create the mid level datum we will again map it on the x y plane and we will offset it in the z direction by 35 millimeters okay let's rename it and finally the top one click on an empty space to dismiss all the selections and finally we will create the top one mapped on the xy plane offset it by 45 millimeters hit ok rename it and we're pretty much done getting back to our example file we can see that the first step is to create the base or the screw level base of our geometry so let's just hide for a second these two datum planes let's select our sketch we will pad it and we will choose the up to face option the face that we want to target is essentially our screw level datum and select that hit okay and because we've the choose the up to face option we can now select we can now control the height of the pad by controlling the height of the screw level datum like this if we alter the position in the z direction of the datum hit ok you can see that the pad updates accordingly let's reset this to 5 millimeters i will press q on my keyboard i will choose the shadow display then select the loft press ctrl d on your keyboard and we will give it a shape color that we kind of like by pressing again the shadow draw style icon we can alter the direction of our shadow and the other properties of the shadow display mode can be am altered by selecting the file name and going down here and modifying the values that you're interested in press escape in order for the light direction to be registered getting back to our example file let's hide some stuff here so we can have a clearer view of what we are doing we've done the initial pad and now we need to create the loft of the main geometry this loft is controlled by three sketches that are mapped on our crew level datums dot on top and midplane datum so let's try this i will select my screw level datum i will create a sketch and for this one i will use the carbon copy tool select this icon here and then select the sketch that represents the base of our geometry let's hide this datum to have a clearer view of what we are doing we can choose the wireframe view and now this sketch is tied to the dimensioning of the sketch that we have copied using the carbon copy tool close this sketch let's switch to shadow mode we will select the mid level datum let's make it visible select the mid-level datum create a new sketch and again using the carbon copy tool we will copy the geometry of our base sketch but in this case although we copied the the geometry we need to modify the dimensioning so i will hide for a second this datum plane let's switch to wireframe view to modify the dimensioning of a carbon copy and sketch we need to delete this constraint and this one also i will give this edge here a dimension of shift h 40 millimeters and this arc here will have a radius of eight millimeters so shift r on your keyboard eight millimeters and we are pretty much done close this gauge at this point we need to create the sketch that represents the top of our geometry this less sketch is mapped on the top datum and if we open it we can see that it is a circle that is made of eight separate arcs the reason for this particular geometry is to help the loft the additive love tool to be successful in order for the additive love to work correctly it needs to work on sketches that have the same number of vertices so with this in mind let's get back to our file we will select the top level datum and we will create a sketch on it let's start by creating 8 separate arcs always taking care to hit the center of our sketch vertex so one two if when closing the arc you hit a redundant constraint let's select the last one delete it zoom in here right click to dismiss the tool select the two vertices and use the coincident constraint with this done let's switch to the construction geometry and we will create some geometry that helps with the symmetry of our circle by taking care of hitting the correct vertices and let's just hide this datum plane for a second we will create these four construction lines let's select them pressing e on the keyboard we will make them equal select the first one shift d on the keyboard for a dimension of 10 millimeters now select one of the arcs shift r on the keyboard for a radius constraint and we will give it a 14 millimeters radius i will create a construction rectangle right click to dismiss the tool select the two edges press e on the keyboard for a quality constraint and then let's make it symmetric by selecting the outer vertices and the center of our sketch then press s on the keyboard and we have a symmetric rectangle now what we need to do is to select this vertex and this line and press shift o on the keyboard for a point on the object constraint then by selecting this vertex here and this vertex here and the vertex on the construction rectangle press s on the keyboard for a symmetry constraint now for the other three arcs remained here it is enough to select this vertex here this vertex here and this one here press s on the keyboard and we have the symmetry constraint you can see that slowly the the already constrained geometry is highlighted in a light green let's do the same here press s on the keyboard and this one and we have a fully constrained sketch the radius of our arcs controls the overall radius of the top of the geometry and this dimension here the 10 millimeters if we look at our example file will control the overall width of the side fillet on the dome getting back to our file close the sketch and to this point we essentially define the free sketches that we'll create and will be the basis of our additive loft we select them then press this icon here we can switch to shadow view let's switch off transparent preview and preview and we can have a better look on our geometry press ok and we see that there is a big difference in the geometry that we obtained here and the geometry of our example file this is because the positioning of our mid-level datum is different if we take a look at the attachment offset the mid-level datum is placed at 35 millimeters if we move it to 30 millimeters you can see how the curvature of the geometry changes and i will modify also the radius of the base of our dome so if i go into our original sketch and let's make this radius here eight millimeters close this will also trigger a update in all the other sketches that use the carbon copy option okay so with this done let's get to the next step so in our example file i will highlight this pocket here and this is essentially the pocket needed for the screws on the screw level getting back to our file i will create a new sketch on the xy plane hit okay close this sketch we will create a pocket show preview i want it to be through all and reversed hit ok and we have the first set of pockets onto the original file the next step would be creating the center hole let's try to do this so getting back to our file i will select the top level datum let's create a sketch the next step would be creating this relief pocket here and let's get back to our file if we switch view from the top view i will select my top level datum i will create a new sketch on it i need to import some external geometry and notice how importing this circle here will essentially import some b-spline geometry i'm not interested in this to remedy i will import directly some sketch geometry from our first pocket let's switch to the wire frame height for a second the geometry we see that we used this sketch for our first pocket for the screws i will make it visible and i will import this external geometry so i will use the slot tool [Music] let's take a look at our geometry and i think we're pretty much clear so we will close the sketch let's move to perspective view shadow mode we will make this datum plane visible selecting the sketch let's create a pocket i will choose the up to face option and i will select the datum plane as the face to be targeted we will hit ok let's hide the datum moving to the top view we see that we need other three slots to create these we will use a polar pattern so selecting our less pocket let's do a polar pattern we need three occurrences on a 180 degree radius what i want to do also is to reverse the direction hit ok let's switch to perspective view now taking a look at our example file here we see that what's left to do is to make the relief slot and this geometry here for the screw that will tighten it let's get back to our file and we will create a new datum plane this time we will map it on the xz plane and we will rotate it by 45 degrees around the y axis hit ok select the newly created datum plane and we will create a sketch on it i want to create a circle and give it a radius of 3.7 millimeters so shift r and we will place it in a convenient place close the sketch pocket through all and symmetric to plane hit okay expand the less the created pocket select the sketch we will create a pad again symmetric to plane [Music] and this should be 15 millimeters hit ok let's switch to perspective view for our next step i will select this face here and using the hole tool i will choose the isometric profile and a m3 thread dimension hit ok now again i will select this face here and although not really recommended i will map a sketch on it so close this sketch let's pocket for 3 millimeters hit ok for our last step we will create the relief so select the datum plane create a new sketch i want to pocket for 1 millimeters and symmetric to plane hit ok and we have our relief in the geometry let's select this edge here we will choose fill it let's do the other ones this one here this one here also and luckily we have no problems hit okay now let's do this one and this one and we will create a chamfer one millimeter hit okay i hope this wasn't too confusing thank you for staying till the end if you appreciate my work please consider supporting me on patreon and i'll see you in the next one

Channel: OficineRobotica

Views: 1,733

Keywords: freecad, partdesign, realthunder, linkstage3, 3dcad, free, cad, opensource, development, fusion360, alternative, modelling, 3dprinting, 3d printing, assembly3

Id: z9WubShaR3I

Length: 18min 26sec (1106 seconds)

Published: Thu Nov 25 2021

Reddit Comments

[u/ruiseixas]

Hi, did you use Assembly for that?