free solidworks tutorial-loft
type : tutorial ebook - PDF
whats in for audience: lesson to exercise solidworks loft
target feature of tutotrial: solidworks loft
features used in tutorial:
- solidworks sketch
- solidworks flex
- solidworks refrence geometry
- solidworks base extrude
difficulty level: advanced
provided by: SolidWorksAdvisor (SWA)
price: free solidworks tutorial PDF book
or read the tutorial here:
You will create this hammer head during the tutorial :
In this tutorial I assume that you know the basic of solidworks and you should know how to interactively work with the software . this means that you should know how to open a sketch , define a plane and … . if you don’t know the basics I recommend you to visit the solidworks beginner tutorials first.
If you had any questions don’t hesitate and ask me . I always will be there for you .now go ahead and start designing with me my friend .
Its very simple and just take a few steps to complete so stay focused . first select the front plane from feature manager design tree on the left side of your screen . left click on front and it will become blue just like the bellow image :
You can choose the plane directly from the working environment :
The selected plane will look like this :
Now click on the sketch tab from command manager and click the sketch to open a sketch on the selected front plane . when you click on the sketch button it turns to ‘’exit sketch’’ :
Press the spacebar and from the orientation window choose ‘’normal to’’ . sketch a rectangle and dimension it like the bellow picture .
Click ‘’exit sketch’’ to exit the sketch . press spacebar and choose ‘’isometric’’ from orientation window . just for more clarification , hide the planes that you don’t need . right click on ‘’right plane’’ and from the menu that just appeared choose hide (the glass icon on the top) .do the same for ‘’top plane’’ . now your work should be like this:
To make a loft you need to have different sections and for having different sections you need to define planes .Define a plane parallel to front plane .Choose the features tab from the command manager .
On the right , click on ‘’reference geometry’’ and choose plane .
The plane window will open on the left . the ‘’first reference’’ box is light blue which means that you choose the first reference for you plane .
From the feature manager design tree or working environments choose the front plane and set the 25.00mm for offset distance .
If your new plane is on the other side of the front plane just check the flip option to get the bellow result:
Click ok and now you have your new plane :
Plane1 also will be shown on feature manager design tree :
Ok…now we are ready to draw our second section for the loft . select the plane1 and open a sketch on it ( if you forget how to open a sketch just see the page 2) . press spacebar and choose ‘’normal to’’ . now draw a circle and define it just the following picture .
Exit the sketch and see your work in isometric view (press spacebar and choose isometric).
So far you have two sketches on two planes. When I was learning solidworks years ago , I used so many tutorials just like you for trining . tutorials are good for learning but there is something wrong about most of them . they tell you how to do this and how to do that and finally you see that you have created something during your work . but the point is that you didn’t think a little to complete your job . you just followed the instructions so you feel that you need to read the tutorial over and over again to deeply understand the procedure . so what we should do now?!
I’ll tell you . the purpose of this ebook is that you understand the solidworks loft feature . so we focus on loft and I don’t repeat what you just learnt so far . we need three more planes to sketch on . I suppose that now you know how to do it .
To make the first loft , define two other planes .first define the plane2 at the distance of 25mm from the plane1 and then define the plane3 at the distance of 40mm from the plane2 . Examine your result . it should be like the following picture in isometric view .
if your work looks like the picture go ahead and if not check your planes .choose the plane2 and draw a circle on it .this time we don’t use smart dimensions to fully define the circle . select the plane 2 and open a sketch on it . go to normal view .click on the origin and drag the mouse to create your circle. Click on the corner of the square when your cursor changes like this :
Click ok and now you have a fully defined circle . you just add a relation between the circle and the corner of the square which defines the radius of the circle . now exit the sketch and go back to isometric view by pressing the space bar and choosing isometric from orientation window . your design should be like this now :
one more sketch then we can get the first loft . select the plane3 . open a sketch and go to normal view . the final sketch is just like the previous circle so we have two options , we can draw a new circle again or we can use ‘’convert entities’’ to get the circle .
You just draw a circle in the previous step so let use the ‘’convert entities’’ . this tool captures the shape of different part of your design and makes a new 2d sketch for you .
Click “convert entities”
And then click on the last circle (which is grey now) that you just draw . the name of the entity that you selected is shown on the blue box and the circle becomes light blue . click ok . now you have a new fully defined circle exactly same as the last one.
Exit the sketch and once again go to isometric view to see what you did so far .
Now we are ready to make our first loft . we have four different sketches in four different planes . sounds great to make a solidworks loft feature . just check your final isometric view with the following picture and if anything seems wrong examine your work .
click on the “lofted boss/base “ in the features tab .
Loft window appears on the right . in the “profiles” section you must select the sketches that you want to join . by selecting each sketch its name will be added to the list of the blue box . go ahead and select the sketch1 on the front plane . you can select the sketches from the tree or you can select them directly from the working environment . just click on the sketch1 and its name appears on the list and the square becomes blue . Now for the second section of your part select the sketch2 on plane1 . this will add “sketch2” to the list .
If you don’t see the preview of the loft then scroll down to the bottom of the loft window and at the “options” tab check the “show preview “ .
Now you can see a preview of the loft :
The green points on the sections allow you to change the curvature of the loft . feel free to move them . left click and hold on every green point that you wish and then drag it around to get your desired shape .
Now select the sketch3 and sketch4 respectively and get the result shown below:
Click ok and make the first loft . by creating a loft your sketches will hide automatically .
Now we have the first part of our design and for the second part we need one more sketch so you should define a new plane . you should be able to do it now . just select “front” as the first reference and set 200mm distance then check “flip” to get the result shown below :
When you’re done with new plane (plane4) your feature manager design tree should be something like this:
Open a sketch on the plane4 and draw a rectangle like this :
Exit the sketch and run the loft command once again . click on the sketch that you just draw and for the second profile click on the end face of the loft1 to get the bellow result:
If your result is twisted don’t be afraid!! Just left click and hold on green points and move them until you get the desired shape .
Hide the plane4 . right click on it and choose hide .
Ok…now you must have the part shown below and only one more step left to go.
Now we are going to bend the part . at this point we are done with loft so you can take a breath!..we use the “flex” feature to get the final result that we need . it’s a funny feature but you can’t find its icon in the features tab .
So how do we run flex?
As a friend I recommend that you pay more attention to the menus of any software than its icons . this way you will understand the procedure better than just clicking on easy icons. You will find how the software operates and how different features are separated .
Train it now . move your cursor over the solidworks icon on top left of the screen and a menu will pop to the right . now mouse over the insert tab and its menu will pop down . these are all the things that you can insert to your model .take your time and examine them a little .
In the insert menu mouse over the features and from the final menu select flex .
And flex window will open on the left .
Click on the part and a few things happen . first , “loft2” will appear in the blue box of “flex input” . second , two trim planes and a “bend axis “ will show up on your part . the initial shape would be like the bellow picture and we are going to change it .
The part will bend between these two planes and around the bend axis by the angle you specify but the “trim plane 2” is not our desired plane at this moment so we must change its location . click on the box bellow “trim plane 2” and it turns to blue so you can select the position of the trim plane 2 .
Mouse over on the center of bend axis and select it .the trim plane 2 location changes . now set 35 for the angle and set 300 for the radius in “flex input” .
Now you should have the same result as I pictured for you below and if you don’t , just get back and check the inputs .
Ready?! Press the inter and you are done . congratulations , now you have your hammer head .