Tutorial; Multisolid as a way of modelling complex shapes in FreeCAD LinkStage3 dev. branch.

hi to all how is it going so i came about this reddit forum post where dop has asked how to do the strangely shaped internal pockets with freecad so i decided to give it a go the original tutorial is a mastercam tutorial and can be found here at this webpage and for this particular uh tutorial i'm using real thunders link stage free release 10.15 and it can be downloaded from this webpage so as we've said the difficulty with this model is modeling the internal pockets that need to have a constant depth that follows the the external contour of our model so if we take a look at the wireframe you can see that the bottom of the pockets is parallel with the top of our model uh here so let's take a second and by taking a look at our model let's try to find some major geometry elements that can drive the shape and dimensions of our model we can clearly see that we have a outline that we can represent with a rectangle we we have four outer arcs and the center of our model can be represented by two circles let's create a new file in part design we will create a new body and a new sketch on the x y plane hit ok we will rename this sketch as master sketch and we will start by drawing the external bounding bounding box of our model so let's select this vertex here this vertex here and the center of our scratch and then by pressing s on your keyboard a symmetry constraint will be applied i will select the top line and by pressing the shift h on the keyboard i will give it a dimension of 140 millimeters i will select this edge here and pressing shift v on the keyboard i will give it a dimension of 40 millimeters and this way we have essentially represented the external contour of of the model now i want to have some construction geometry for the centers of the four holes in our model so i will do just that i will change to construction geometry by hitting this icon here on the toolbox let's choose the rectangle tool let's create another rectangle right click to dismiss the tool select the two outer vertices and the center of the sketch press s on your keyboard for a symmetry constraint now we will use a little trick to represent what it is essentially the radius of this outer arc here so let's get back to our drawing i will create a construction rectangle that is constrained to these two vertices this one here and this one here okay i need it to be an actual rectangle so i will select these two edges press e on the keyboard for a equality constraint now select this edge shift h on the keyboard for a horizontal [Music] dimension and we will make it this eight millimeters so uh to this point we have essentially drawn the outer perimeter of the model and we have the centers of the four holes that we have here we will actually draw these holes so i need some regular geometry let's change to regular geometry we will create some circles and by taking care of hitting the vertices i will create a circle that will be tangent you can see that the solver will automatically add a tangency constraint if we are over the top edge so this circle will will be tangent to the outer perimeter of our geometry and we will do four three others that need to be tangent [Music] and notice how we have a fully constrained sketch using only three dimensions now i would like to represent these this part of the center part of the geometry and i will represent it with two other circles so always two regular circles let's hit the center of our geometry i want the outer circle to be tangent to the external of the geometry and the inner circle to be tangent to this construction geometry rectangle i will use the polyline tool to create some geometry that will turn useful later uh in the process of modeling so right click to dismiss the tool i will do the same under so the points need to be attached to these circles and by selecting this line and this circle and pressing t on the keyboard i will give a tangency constraint between the circle and this edge here i will do the same for the other three left so select the edge and the circle t on the keyboard for a tangency constraint again here t for a tangency constraint this one here t for tangency constraint and we have this vertex here and this vertex here fixed on the inner circle but i want them to be also fixed on the vertical sketch axis so select the vertex and the vertical sketch axis and by pressing shift o on the keyboard we will constraint uh constrain the vertex so select the other one select the vertical sketch axis shift on the keyboard and we have a fully constrained sketch with this this major geometry elements locked in in our master sketch let's close this sketch and let's see how we can proceed to eventually get to this finished model so let's hide some geometry here and let's go step by step the next logical step for us would be to essentially pad the outer perimeter of the model to do this we will create another sketch always on the x y plane hit ok and we will import some external geometry from our master sketch so using this icon here i will import the four outer circles i know i need them i will also import this circle here now using the r tool i will start to block out loosely the external of my geometry and two on the keyboard by taking a look at our model we can see that we have we can see that our geometry is comprised of two other arcs here so let's go ahead and draw them let's choose the arc tool by hitting the horizontal sketch axis and trying to hit the vertices of our previous arcs we will create this geometry here right click to dismiss the tool now choose the line tool try to hit to be constrained to the to the vertices of our arcs and we will close the perimeter of the sketch a horizontal constraint was automatically added here and we will remove it because it will create some problems if we go ahead let's take a look again at our geometry and we can see that we have some other arcs here that connect the external edges with the center circle so let's create this to do to do this i will use the fillet tool i will select this arc here and this edge here i will select this arc here and this edge here and we have the fillets this one and this one and this one and this one notice how the arc tool creates uh automatically creates some nice tangency constraint constraints between the edges we will need to do these constraints manually for the other other edges so select this geometry and press t on the keyboard and you will be prompted uh that a tangency endpoint tangency was applied applied and we will slowly go ahead and do the same for the rest of the sketch where the tangency constraint is missing so now what i want to do is to have this arc here and this arc here equal and i need to import some other geometry here i need this line here and this line here also and now it is time to constrain our sketch to the dimension dimensions from the original master sketch i will choose this art here and this circle here and we will make them equals by pressing e on the keyboard let's do the same underneath it so e on the keyboard and we will do the same for the four outer arcs select this one and this one e for equal now we can give our radius to this arc here so shift there are on your keyboard for a 15 millimeters radius we will select the these four arcs here and press e on the keyboard for a equality constraint i will give them a radius of shift r 30 millimeters and we need to constrain this vertex here to this line so select the vertex then the line and shift o on the keyboard for a point on object constraint we will do the same with the other ones so shift o on the keyboard select this vertex here this line here shift o this vertex here and this line here shift all and we have a fully constrained sketch that represents the outer perimeter of our model and i think we are missing the center circle we don't have it so we will import this geometry use the circle tool let's create a nice circle select this external geometry and our circle e on the keyboard for a equality constraint let's close our sketch and test to see if we modify the dimensions in our master sketch if we don't break the model so let's try 140 millimeters here 50 millimeters here close the sketch and as you can see our model outline follows the dimensions dictated by the master sketch let's close this let's get back to our original dimensions so 103 30 40 millimeters close and now all that's left to do is to pad our sketch so let's pad it for 15 millimeters hit okay and we're pretty much done at this point we can select our body press ctrl d on your keyboard let's choose aluminum as material i want a shape color something like this and we will play a bit with the material properties here i will make it a bit more shiny so let's try 15 the specular color needs to be something a bit bright close this one close okay because we're using link stage 3 we can choose the shadow display mode select the name of your file i want a ground transparency transparency of one and we're pretty much set it up okay so now on to the next step what we want to do is to create this slope here on the model and to do this we will use a revolve cut so getting back to our model select this circle here and we will create a datum plane i want to rotate this datum plane around the y-axis by 90 degrees and also around the x-axis by 90 degrees hit okay and you will see why i rotated the datum plane this way in just a second so select the datum plane i will create a new sketch i will import this external geometry and by using the polyline tool i will essentially create the shape that will that we will use to create the slope on our model right click to dismiss the tool by using this icon here we can rotate the view to be aligned with the with our sketch select these two vertices here and shift v for a vertical constraint of three millimeters and i don't know why this one this vertex here should be coincident with this vertex here okay let's close the sketch hide the datum plane and using the revolve cut and the base z axis we will cut our model as you can clearly see the the sketch was not enough to do a clean cut so let's make sure that it is correct this time okay so this concludes the creation of the of the sloped part of our model let's see what the next step would be so the next step would be creating the four holes for our model let's get back to our file let's unhide our master sketch let's hide the model for just a second so select [Music] these four circles here unhide the model what i will do now is to create a pocket reversed through all and the important part here is to give it a feed tolerance because we essentially need only the center of our four holes let's click okay select the geometry of our four holes and we will use the hole tool i want the profile to be a isometric one i want the size to be a ms6 or eight i think and i want a dim standard hole type click ok and we have this way our four holes okay let's hide the master sketch for just a second and now we're getting into the part where we need to create the two internal pockets to do this we will use some boolean operations and these are offered in link stage 3 directly in the part design workbench we will start by creating the geometry for that will define the shape to be cutted from our main body piece one thing that i will do now is to activate outer solid group what this will do if you take a look will uh revert the order of the treeview with your latest feature at the top and we will take advantage of the possibility in link stage 3 to have multiple solids inside inside the same body we will create a new sketch we will map it on the x y plane hit ok and let's hide our geometry for just a second we will unhide the master sketch and i want to import some external geometry which will be this one this one and this one i want to create two arcs that will be tangent to our circle here another arc here by hitting the center of our sketch i will create another arc here and a connecting one here let's apply the tangency between this one so select the two arcs press t on the keyboard let's do the same here t on the keyboard okay and using the line tool we will connect these ones here okay i need to import some other geometry so select this one and this one select this edge and this geometry here and we will give it a parallel constraint and we will do the same under here so parallel constraint and what i need to do is to have this vertex here and this vertex here symmetric to the horizontal axis of our sketch so select the two vertices the horizontal axis and press s on the keyboard for a symmetry constraint let's close our sketch and we need to move it up by 20 millimeters so select the sketch we will expand the attachment to offset in the position field we will move it by 20 millimeters in the z direction now select the sketch let's pad it reversed and the important thing here is to make the operation as a new shape i will unhide for a second our geometry and this for dimension i want to pad it for 17 millimeters hit ok and we essentially have the shape that will cut our internal pockets now i want to select select our pad and bear in mind that this is a separate geometry a different solid in respect to our geometry that we've done previously so let's select our pad we will create a mirrored feature hit ok we will hide for just a little bit the geometry here let's hide our master sketch i will select by pressing ctrl on the keyboard these edges here and i will create a fill it with the radius of six millimeters hit okay now let's unhide our master geometry i will create a shape binder that we will use to cut this geometry here so let's select this face here this face here and this basically here and we will create a green subshape binder now there is a really important step that we need to do here in order to for our successive operations to succeed and we need to set the fuse property of our shape shape binder to true this essentially will make so that the geometry kernel inside the freakhead will treat the geometry of our shape binder as a unique contiguous shape and can be successfully used to look at our geometry i will unhide the geometry of our fillets i need to move or offset the position of the shape binder and by expanding the placement property position in the z direction i will offset it by 7 millimeters okay now select the binder select by pressing ctrl the fillet and we will use the split operation so hit the split operation and we will activate this geometry here that we need that we need in order in order to have the two pads in our model let's tweak a little bit the position of our binder i will now proceed at creating some fillets so select these two edges here and let's create eight millimeters fill it hit okay and now i want this face here this face here so essentially the bottom of our pads to be filleted perhaps five millimeters hit okay let's unhide our main geometry i will select first the fillet then the geometry of the whole and we will do a boolean operation and let's set it to cut and voila we have our complex geometry that follows the slope the external slope of our geometry so let's switch to wireframe and we're pretty much done hit okay let's switch to shadow perspective view we need to hide the geometry of the whole and that's pretty much it one question that i was asked how i set it up called per face colors for the model so we can select the faces that we're interested in by holding down control then right click on the last feature of your tree view set colors and a dialog will be open open it to set the colors for those particular faces let's hit ok and we're pretty much done thank you for staying till the end it was a long one and i hope to see you really really soon

Channel: OficineRobotica

Views: 19,584

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

Id: C2w0BV_j5Mo

Length: 25min 21sec (1521 seconds)

Published: Tue Nov 02 2021

Reddit Comments

[u/justacec]

u/OficineRobotica ! Thanks for the tutorial. This looks great. I have been wanting to switch over to the LinkStage but I was nervous as I am in the middle of a large project and wanted to wait. But this looks great. Thanks again for the tutorial. Always love your stuff.

[u/mranderson17]

Hey, great video! I'm glad to see you're back to making your tutorials, I find them to be the most comprehensive when it comes to the features available in realthunder's LinkDaily fork.

I would have never thought of doing a pocket with a small fit tolerance to create geometry on the other side of the body without an additional sketch. That's a really clean way to get a base for a hole without a lot of extra work. I'm going to be using that a lot now.

[u/Marthinwurer]

Man, at what point does RealThunder's branch become a fork?

[u/MannyTank]

I'm a complete noob using this software and to CAD in general. I always run into the issue of taking the complex route, or over constraining my sketches. The way you did this so clean definitely gave me some good ideas and future practices on how to approach things in the future. My respects and thank you for the insights.

[u/JustEnoughDucks]

Great tutorial! how did you get your UI setup like that? It looks much better than the default!