FreeCAD 0.19 - Tutorial - Simple Part with Part Design (EN)

hello and welcome to this new freakit tutorial here on the freecad academy the simple part with part design that's a tutorial officially released in the freecad documentation in the freecad wiki to give you some extra value from this video i will divide this video into two parts in the first part i will model the tutorial exactly as it's in the documentation i will do all the steps that are described there then i will show why in my opinion this is not the optimal way of modeling a part in freecad you should have heard of the topological naming problem or toppo naming and the techniques used in the tutorial in the documentation don't take care of this problem and so we will have some issues so i developed a workflow that's more stable considering the topo naming problem and i will compare these workflows let's model the part according to the documentation freecad 19 new file part design workbench create a new body create a sketch create the sketch on the x z plane and then let's start drawing as you know i like to drag and drop a little bit to the bottom left to have more space for my drawing i start with the polyline tool make a little vertical line angled line a horizontal line then polyline extra power triple m on the keyboard to make it an arc go down a little bit and close the shape right click to quit the command first thing i'd like to do is to fix the corner point here onto my sketch origin point by using the coincident constraint let's have a look which other geometric constraints are missing this line here is vertical but not in my sketch as you can see i can drag and drop this line and it will not stay vertical so we have to select it select the vertical constraint and that's it let's continue with dimensioning we have 50 millimeters from this point to this point in vertical distance and in horizontal distance as well everything according to the original we have a total length of 100 millimeters down here we have the radius of 20 millimeters up here and then there is still one degree of freedom left and that's for example the angle of this line so let's select these two lines here angle 30 degrees fix this little dimension a little bit make it better visible for you and then the sketch is complete i close that now i'm back in the part design environment sketch is still selected so i can select the pad command here from the tasks menu 30 millimeters okay so that was the easy part of the tutorial we need to make a hole in the middle of this face here the first suggestion from the original tutorial is to select this face and click on new sketch caution this is something i do not recommend placing sketches directly on faces as you might know from my other videos but i will do it now because it's shown in the original tutorial so the next step in the original tutorial is to link these two edges here from the 3d body to make it better visible i press and rotate in my sketch so i can see the 3d body i click on create an edge link to an external geometry i link these edges here that's another thing i do not recommend doing and then i create two lines make them construction lines from this point to this point here another line from this point to this point here make sure the point is properly selected then you will see across here switch over to the sketch geometry create a circle that's fixed on this line for example make it 10 millimeters in diameter and now the last thing we need to do we also need to fix the center point of this circle to the other line here and now it's fixed in the middle close pocket through the whole body and that's cool that's the method shown in the original tutorial in the wiki and if you're an experienced viewer here on my channel you will know that this style of modeling is very dangerous in freecad so watch out so let's break the model it's pretty simple to break it all we need to do is to enter the first sketch here this basic shape and why not change this radius here and instead make a chamfer so we can set this radius to construction and close the now no longer closed shape with a chamfer something like that so now we no longer have this radius here but a flat surface on this side i close this one is still working pretty good so i have not broken it yet the two correct edges are still linked therefore we need to change sketch number one a little more we make a little radius here constraint preserving fill it set the fillet for example to 10 millimeter the angle somehow disappeared so we have to set it again 30 degrees and that's it so let's close it and see what happens yup not so funny as you see now the drill here left its original face on the top of the model and is now located here when we enter the sketch you will see that the sketch is no longer fixed on this face here but on this let's go back go back to sketch number one let's put this line to construction mode and this line to the regular mode see what happens now now the drill is placed on this face here so it's somewhere completely different so no matter what we do whenever we change or even make small changes to our original geometry something really weird is going to happen there so that's another good example for the topological naming problem and a good example why i do not recommend this style of working so next part of the video how can we fix it the first thing i need to know i delete the complete pocket and i leave this complete sketch here this is not optimal for me i delete the sketch now i enter the first sketch um i make it look like the original sketch again this is a little bit of work to do for me but not too hard i connect this two points again i have the radius 100 50 50 30. everything is very fine now still padding of the first sketch i would not have padded 30 millimeters in y direction i would have said symmetric to plane because it's a symmetric part and working symmetric is always very welcome for these parts okay and now we still have to make the hole there on this surface as i told you we do not select 3d surfaces for sketch placement so we have to find a different method and my favorite method is going with parameters i open the sketch and this parameter here that's defining the height of the whole model double click name optional name i name it z underline total and then we need to take care of the placement of the hole and the hole is always located here in the middle of this line here so i draw in a construction line go to construction mode new line from here down here select it make it vertical very important and then i need to say that these two points and this line are symmetric so i have now this little construction line here in the middle of the face and now i need to have the distance from this point to the sketches origin so i select a horizontal distance the sketch is already fully constrained so we cannot define any more driving constraints be careful so we need to select these two points and before we kill the sketch we have to select reference because this is only a reference dimension this is not a driving dimension so and now let's call it z underscore hole okay and okay close it next thing to do is create a sketch i make the xy plane okay i enter the section view and i draw a circle that's fixed here on the horizontal axis diameter 10 millimeters and now i need the distance from this point here to the sketches origin point i select both i go to horizontal distance now i don't enter a length but i click here on the formula editor now i'm in the formula editor i can access the z hole parameter that i defined in the other sketch i enter the brackets sketch dot constraints dot z underscore hole we see 65 millimeters displayed here as the result okay okay now it's in pink color so that means that this is a reference dimension very nice close now we still have one problem this sketch is down here on the bottom um i would like to have the sketch on the upside here of my part therefore i select sketch number zero zero one let's rename it it's i don't like this i call it sketch hole and the other sketch is now renamed to sketch profile okay so let's continue i select a schedule i look down here in the properties of the sketch attachment position and in z direction as i go to the formula editor again in the formula editor i now can access the new name sketch sketch profile constraints and now it's z underline total because that was the name that i gave the total value of z and as you see the sketch is now located on top of my geometry and i can use this sketch for a pocket command here through the whole body okay that's cool that's working but i don't know if it has an advantage yet because i haven't tested if it's stable towards the topological naming problem so i have to do weird things in the sketch profile and change it so the first thing i did was to change this one here to a construction line and fill in here a line let's make it a little bit more confusing this time we go with the polyline and why not entering even more lines so something like that let's give an angle here 135 degrees and we have one degree of freedom left so let's give a dimension from here to here of 12 millimeters now the the shape is going to look very transformed but we don't care all we want is that the hole is still in the right position right so let's close it and looks pretty stable to me so let's change it even further the sketch profile now we get really crazy we select this point here to make a constraint preserving sketch fill it on this point here watch out the angle was deleted again to set the correct angle here 30 ml 30 degrees i always want to say 30 millimeters and let's define a crazy radius of 20 millimeters close it and still the pocket here is not affected it's in the right place it's still working very well so let's set the tip to the pad set tip so we are in the construction history we are at this point and we even change worse things we select these two edges here and create a 3d fillet filleting on edges seven millimeters and now let's change the tip again to the pocket set tip and it still looks like it's still working correctly even when we place the fillet in the modeling history before this pocket here these are all things that would kill models that are vulnerable to the topological naming and now let's do one last thing so let's further change some values here 25 degrees 40 millimeters and 5 and degrees and the total length of 100 and maybe 20. so now we change it a lot in the model let's close and see what happens the hole in this face here is still in the perfect position we can even change the dimension of the first pad make it wider but the hole is still fixed in place here in this i hope this was a good proof to you that this model is rock solid stable i hope you enjoyed the video i hope you see some extra value for you in this video compared to the original tutorial in the wiki i hope you had a good time here in the freecad academy stay safe and see you next time goodbye my friends

Channel: FreeCAD Academy

Views: 14,148

Keywords: Freecad 0.19, free cad 0.19, cad, free cad, Freecad part, Freecad part design, free cad part design, cad design basic, cad design basics, Freecad wiki, Freecad documentation, Freecad help, free cad help, free cad documentation, free cad wiki, Freecad basic tutorial, learn Freecad, flowwie, flowwies, floppies corner, cad education, Freecad beginner, Freecad newbie

Id: FVKhejma69U

Length: 17min 58sec (1078 seconds)

Published: Sun Aug 01 2021

Reddit Comments

[u/flowwstar]

How do you like the new video 😄