we're going to compare the differences in workflow between on shape and freead to model this simple part which is a bicycle seat clamp it'll be a straightforward modeling process followed by an assembly you might be surprised by the result on the left the part will be modeled with on shape and on the right with fread you can follow the video as if it were a beginner's tutorial before we begin the comparison let me know in the comments which software you use and why the video is divided into chapters so you can go directly to the sections that interest you we will do a quick comparison between the two software after each step and you'll find a full summary at the end you will also find the 3D files for the tutorial in the description you can download them for free on my Kofi page or make a donation if you want to help the channel grow thank you in advance let's start with on shape the interface May differ from yours because I had to resize it to fit the screen to create a sketch you first need to select a plane and in our case we choose the top plane so left click on the top plane then click on the sketch icon in the top menu to make it easier to draw we'll click on the word top on the navigation Cube to align the view perpendicular to the sketch plane we'll start by drawing two circles at the origin point to do this go to the top menu where the line icon is then click on the small Black Arrow to select the circle tool then left click on the center point of the plane and move your mouse to enlarge the circle then left click to confirm the drawing and type the dimension of the circle which will be 39 mm repeat the same operation to create a 34 mm Circle we're going to draw the rear part of the clamp to do this go to the sketch geometry menu click on the black arrow and select the line tool start with a vertical line to the left of the circle by left clicking to begin the drawing then make another left click to connect the line to the circle press escape to stop using the tool repeat the same drawing but this time below the axis you can use the Symmetry tool if you want but when it's just a few lines like this it's sometimes faster to recreate them press escape to stop using the tool now we're going to apply constraints to fully Define our sketch we'll start by making the lines that touch the circle tangent to it to ensure a smooth transition between the circle and the lines to do this simply select the line and then the circle without holding control then go to the constraints menu click on The Black Arrow and find the tangency constraint repeat the same operation for the bottom line next select the two small lines on either side of the axis and apply an equality constraint by clicking on the equal icon in the constraints menu now let's apply Dimension constraints go to the top menu and click on the dimension tool you can select the two points on either side of the line or just the line itself to apply a dimension give a dimension of 8 mm still using the dimension tool give a dimension of 28 mm between the center of the circle and the point at the far left to avoid multiple Contours even though on shape can handle it we will delete the Arc of the large circle on the left so that we only have one contour to do this we use the trim tool to remove that part of the line click on the trim tool in the top menu then click on the part of the circle you want to remove the sketch is now complete we can exit it by clicking the green check mark at the top we're now going to extrude the sketch's Contour to give it volume to do this first select sketch one in the left menu then click on the extrude icon in the top menu in the menu that opens you can leave the default settings and just change the depth to 14 mm this will extrude the Contour over a distance of 14 mm note that in this menu we also have several options such as the ability to create an extrusion that removes material we can confirm the operation by clicking the green check mark at the top we can hide the three planes by clicking on the IE icon in the left menu we've completed the first Extrusion operation now let's see how this process works in freecad before starting the modeling in freecad make sure you are in the part design workbench to create a sketch click on the sketch icon in the top menu freead will ask you to choose a sketch plan to draw on select the XY plane which corresponds to the top plane in on shape and left click on it you'll notice that unlike on shape the 3D view in freead automatically aligns perpendicular to the sketch plane allowing you to draw Flat just like on a sheet of paper and on shape you have to manually adjust the view you can change this setting in freead if you don't like it we'll start by drawing two concentric circles with their Center at the origin to do this click on the circle tool in the top menu then left click to place the center of the circle on the origin point you can then move your mouse to enlarge the circle or directly enter a diameter value in our case type 39 mm and press enter to confirm still using the circle tool repeat the same operation but set the diameter to 34 mm at this point you should have two concentric circles in green now we're going to draw the rear part part of the clamp to do this we'll use the polyline tool go to the top menu and select the polyline tool start your drawing by snapping to the bottom left part of the circle then draw vertical lines on either side of the red axis and finally connect to the top left part of the circle to stop using the tool right click or press Escape we're going to make the circle tangent to the straight lines that touch it to ensure a smooth transition between the two to do this select cect the line and the circle then click on the tangency constraint icon in the top menu you can uncheck the box in the menu that opens to stop being bothered by this message then click okay repeat the same operation for the bottom line next select the two small lines on the left then click on the equality constraint icon in the top menu to make them the same length all that's left is to add Dimensions to fully constrain our sketch click on the dimension tool in the top menu then give a horizontal dimension of 28 mm between the left Center Point and the origin you'll notice that unlike on shape freead directly suggests a dimension from the origin still using the dimension tool give a vertical dimension of 8 mm now all that's left is to delete the large Arc to have only one contour even though in some cases freead can handle multiple Contours it's always better to have just one to delete the arc simply select the trim tool in the top menu then click on the part of the arc you want to remove you should now have a fully constrained and completely green sketch you can click the close button in the task menu to exit the sketch now we're going to turn this sketch into a solid by performing an extrusion in freecad this operation is called a pad to do this make sure sketch is selected then click on the pad icon in the top menu in a menu that opens change the length to 14 mm to get the correct Extrusion height then click okay or press enter to confirm the operation we should now have the same object in both on shape and freecad after this first step what can we say about on shape and freecad initially the workflow between the two software is identical they have the same tools for drawing sketches the same constraint and modification tools however there are a few differences to note on shape has better port for sketches with multiple Contours whereas freead can manage it under certain conditions on shape doesn't offer the option to align the view directly perpendicular to the plane unlike freecad which provides this option that can be disabled additionally on shape requires an extra click before entering a dimension whereas freead doesn't also freead automatically proposes creating a dimension from the origin whereas on shape does not for this first step there isn't much more to say in terms of notable differences we will now move on to the second step which involves removing material from the rear part of the clamp let's start with on shape we will create a sketch on the top face of the clamp to do this click on the face then click on the sketch icon in the top menu align the view perpendicularly by clicking on the top icon in the navigation Cube we will start by drawing a center line that will serve as the axis of symmetry click on the line tool then draw a horizontal line starting from the origin and extending to the midpoint of the left Edge you will notice that on shape automatically offers to snap to the edge press escape to stop using the tool to prevent the line from interfering with our sketch we will convert it into a construction line to do this select the line then go to the drawing tools and choose construction next select the corner rectangle to tool from the drawing tools menu draw your rectangle by snapping to the left Edge then finish the last corner by snapping to the edge of the circle press escape to stop using the tool we will now make this rectangle symmetric with respect to the dashed axis to do this select the top left point then the axis then the bottom left point and click on the Symmetry constraint tool in the top menu the only thing left is to set a dimension for the width of the rectangle to do this click on the dimension tool in the top menu and set the rectangle width to 5 mm the sketch is now complete we can exit it by clicking on the green check mark in the top menu we will now create the cutout first select sketch two then click on the extrude icon in the top menu in a menu that opens select remove instead of add and change blind to through all this creates a cut that goes all all the way through the part you can click on the green check mark to confirm the operation we have finished the cut in on shape now let's look at the procedure in freead start by selecting the top face of the clamp then click on the sketch icon in the top menu unlike on shape we don't have direct access to the edges of solids and freecad we need to project them into the sketch to do this click on the create external projection geometry tool in the top menu next select the left Edge and the circle rightclick or press escape to stop using the tool next select the newly projected lines and convert them into construction Lines by clicking on the construction line icon in the top menu then use the rectangle tool and draw a rectangle by placing the first corner on the left Edge and the other corner on the circle rightclick or press escape to stop using the tool we will now make the rectangle symmetric with respect to the red axis to do this simply select the top right point then the axis follow by the bottom right point and click on the Symmetry constraint tool in the top menu the only thing left is to set a dimension for the width of the rectangle select the dimension tool and set the rectangle's width to 5 mm the sketch is fully constrained we can close it by clicking on the close icon in the task menu to create the cutout we need to select sketch 00 1 and then click on the pocket icon in the top menu next change the type to through all and click okay or press Center to confirm the operation we've completed the second step now let's review the differences between the two software programs we can say that the workflows are quite similar however a big Advantage goes to on shape for its ability to snap geometry directly onto existing solids without needing a projection tool this is a significant timesaver and makes the workflow more intuitive another notable difference is that on shape uses the same tool for both adding and removing material while this requires one extra click compared to freeat it simplifies the user interface by reducing the number of tools needed we will now proceed to the third step creating a slightly more complex and Technical opening to see how the software handles it let's start with on shape the goal of this material removal is to create create a small lip at the top of the clamp to prevent it from sliding down the seat tube we want to ensure a lip thickness of 0.5 mm even if the clamp height changes the objective is to achieve this without using variables to begin flip the part over select the bottom face to sketch on then click on the sketch tool using the circle tool draw a circle centered at the origin with a diameter of 34.9 mm which corresponds to the diameter of a bicycle seat tube click on a green check mark to close the sketch next select sketch three and click on the extrude tool next select remove instead of add in the extrude options and in the drop- down menu choose up to face instead of blind in the viewport select the top face of the clamp we want this Extrusion to stop 0.5 mm before the top face in the extrude menu check the offset distance box and enter a value of 0.5 mm you should see in the 3D preview that the lip has been created properly this technique ensures a constant gap of 0.5 mm regardless of the clamp's height even if we were to change it later let's see how this operation Works in freecad turn the clamp around and select the bottom face then click on the create a sketch icon using the circle tool draw a circle with a diameter of 34.9 mm at the origin of the axis and click the close button to exit the sketch make sure that sketch 002 is selected then click on the pocket icon in the top menu in the drop- down menu for type change the dimension to up to face then select the top face in the viewport and change the offset to face to 0.5 mm then click okay or press enter to confirm the operation for this operation we can note that there are no significant differences freead might require one or two fewer clicks but the workflow is essentially the same we will now create two 5 mm fillets on the rear part of the clamp I noticed that some of you were triggered by the pronunciation of filet the correct pronunciation is fet with the T pronounced and I'll make an effort to use this pronunciation for the rest of the video let's start with on shape select the two rear edges of the clamp and click on the fet tool in the top menu change the radius to a value of 5 mm before confirming the operation I like to point out that in on shape you can set a fet radius larger than the available width and the operation will still succeed try setting it to 10 mm you'll see that it works in our case keep it at 5 mm then click the green check mark at the top let's now see how this works in free cat select the two rear edges of the clamp then click on the fet tool in the top menu set the radius to 5 mm if you try to set a radius of 10 mm you'll see that the operation won't succeed unlike an on shape where the operation works you'll need to find another technique if you want to create a larger fet press enter or click the okay button to accept the operation for this fet operation we can can note that once again the workflow is the same it's not easier in either case the biggest difference lies in the flexibility to create radi larger than the available length with on shape in freecad this operation is not possible and requires finding a workaround or another way of modeling to achieve the desired shape let's now focus on creating custom planes starting with on shape we will now create the hole at the back of the clamp to insert the bolt we could do this using a whole operation but I think it's more relevant here to perform two material removal operations instead select the face on the inside of the back part of the clamp and then click on the sketch tool to create a sketch at that location the goal is to create a circle at the center of this face to do this using the line tool we will first draw a vertical line starting from the center of the bottom Edge and ending at the top Edge next select the line and convert it into a construction line next use the circle tool to draw a 5 mm diameter circle at the center of the line you just created if the circle is in construction mode convert it back to a solid line using the same tool you can exit the sketch by clicking the green check mark next select sketch 4 then click on the extrude tool and perform a remove through all also check the symmetric box so that the operation is performed in both directions click the check mark to confirm the operation so far nothing new Under the Sun let's do the same operation in freead before creating the custom plane select the face on the inside of the back part of the clamp and then click on the sketch tool to create a sketch at that location in freecad you can have a section view while drawing your sketch to do this simply click on the icon in the menu bar this allows you to see exactly where your sketch will be drawn unlike on shape we need to project the edges to be able to snap onto them using the external geometry tool click on both edges to project them into the sketch and convert them into construction lines to prevent them from interfering with the sketch then use the line tool to create a vertical line starting from the midpoint of the bottom Edge next select this line and convert it into a construction line using the circle tool draw a circle at the center of the line with a diameter of 5 mm then click on close to exit the sketch with Sketch 003 selected click on the pocket tool icon then choose through all and check symmetric and click okay to confirm the operation we will now create a custom plane to perform a material removal for the bolt head starting with on shape to do this select an extreme point of the delay like this one and then the interace of the clamp after that click on the plane icon in the top menu the plane has been created exactly at the intended location so you can confirm the operation we will now draw a circle on this plane select the plane then click on the sketch icon in the top menu you can align the view by clicking on the front of the navigation Cube using the circle tool create a circle with a diameter of 8.7 mm you can place it randomly we will constrain it later next select the whole circle and the newly created Circle and apply a concentric constraint the circle should now be in its correct position you can exit by clicking the green check mark next select sketch five then click on the extrude icon in the top menu choose remove then check second end position and enter 4 mm for the first Direction and 2 mm for the second Direction click the green check mark to confirm the operation you can optionally hide the plane for better visibility let's now look at how to create this custom plane in freecad while holding the control key select the in toop point of the fet and the inace of the clamp then click on the data plane creation tool the plane should now be created exactly in the correct position you can confirm by clicking okay next select the data plane then click on the create sketch icon click on the section view icon and by using the external geometry tool select the circle of the hole rightclick or press escape to stop the tool then convert the circle into a construction line using the circle tool draw a circle with a diameter of 8.7 mm at the center of the projected Circle then click on close to finish the sketch you can hide the data plane for better visibility with Sketch 004 selected click on the pocket icon in the top menu change the type to two dimensions and set the first direction to 4 mm and the second direction to 2 m press enter or click okay to confirm the operation you should have the same result in on shape and freead in this case the workflows for creating a custom plane are identical to make the part easier to insert onto the seat tube We'll add a small chamfer on the rounded edge of the bottom face starting with on shape select the rounded edge of the bottom face then click on the chamfer icon give a value of 1 mm then confirm to create a chamfer in freecad select the edge of the circle on the bottom face then click on the chamfer icon give a value of 1 mm for the chamfer then click okay to confirm the operation the process of creating a chamfer is the same in both software to make the clamp more visually appealing We'll add a 1 mm fet to the top and bottom edges I'll speed up the video 3x since it's the same as the fet we created earlier and there is no difference between on shape and freecad let's move on to a small assembly to compare how the two software handle it we will add an M5 bolt and create an assembly with this bolt before starting the assembly let's rename the two bodies to clamp to have a proper file structure let's start the assembly with on shape you need to switch to the assembly workspace by clicking on the assembly tab at the bottom left of the screen start by inserting the clam into the assembly to do this click on the insert icon and select the clam body since we're not caveman we'll generate the M5 bolt directly at the right location in the assembly to do this click on insert again go to the standard content app as I did before onshape has kept my last bold generation onshape gives you the option to generate various types of Fasteners according to their different standards categories and classes in our case case we select ISO bolt and screws socket head screw then hex socket ISO 4762 with a size of M5 and a length of 20 to create your bolt afterwards nothing could be simpler just click on the insert icon at the bottom on shaped generates the bolt and you can directly place it on your clamp by selecting the inner edge of the clamp it's a very fast way to add Fasteners to your assembly as it automatically applies the constraint between the clamp lamp and the bolt let's now see how to do this with freecad first you need to download the Fastener workbench by going to tools and then add manager once downloaded go to the workbench drop-down menu and choose Fasteners this workbench has a vast selection of Fasteners that you can use for your projects you can place bolts directly in this workbench but we will use the assembly workbench to join the clamp and the screw together to ensure that the bolts position updates along with the clamp click on the ISO 4762 Bolt from menu you can see that the bolt has been created in the tree view to change its properties select the bolt and in the properties panel change the diameter to M5 and the length to 20 mm the bolt should update and be positioned at the center of the clamp to continue with the assembly in freecad switch to the assembly workbench which has been added since version 1.0 of freecad to create an assembly click on the create assembly icon in the top menu before continuing with the assembly you need to hide the clamp and the bolt by clicking on the I icon in the tree view then click on the insert component icon in the top menu to import the parts start by clicking on clamp to import this part first freead will automatically ask if this part should be fixed click yes in the menu that appears next import the M5 bolt by clicking on it you can use the parts Gizmo to move the bolt and place it in a more accessible position and click okay to confirm the insertion we will now create a joint between the bolt and the clamp to do this select the edge of the bolt that will be in contact with the clamp then select the corresponding Edge on the clamp while holding the control key then click on the fixed joint icon in the assembly tools menu the bolt should now be correctly positioned on the clamp you can click okay to confirm our two assemblies are now complete what can we take away from his experience the assembly technique is the same between both software however we can note that an on shape adding Fasteners is greatly simplified since we can assemble them directly freeads Fastener library is more extensive but requires installing an add-on which is free a small detail freead asks to fix a part at the beginning of the assembly to ensure that components don't move unlike on shape it's also worth mentioning that freeads assembly workbench is still less stable compared to on shapes so what can we conclude after this modeling and assembly test in summary onshape offers a smoother and more optimized workflow while freecad provides greater flexibility with more customizable tools but the cost of sometimes more technical manipulation but we must consider two important factors price and accessibility on one hand on shape is a paid software costing around 1,00 ,500 for the license or it could be free but with a big asterisk your files must be public and you can't use the software to create pieces for sale you also need an internet connection to model and access your files freead is the complete opposite the software is free and open source you don't need an internet connection and your files are private let me know in the comments what you think about this and which software you use and why I think there's never been a better time to test free cash because as we've seen the workflow is the same as that of paid CAD softwares if you want to learn freead you can subscribe to my channel where you'll find several tutorials showing you how to use freead professionally I hope you learned something from this video or that it entertained you thank you for your attention