3D Modelling in Alibre Design

Welcome, this tutorial is based on Alibre Design version 12.1. For any additional information such as installation, registration or upgrading, Please contact CADDIT.net via email. In Australia a free trial download for Alibre Design Professional is available HERE.

For this section of the tutorial, assumptions have been made that the designer has completed a sketch which doesn't have any errors in it and the analyse tool as accepted that the sketch has no open sections or overlapping areas in the sketch. If you haven't check your model for errors or used the analyse to check for any issues with the sketch, please ensure this is done, otherwise the 3d functions in this section will not work.

Extrude boss and cut

  Extruding step is putting your 2D sketch to a 3D model. There are two steps with this process which can be performed to accomplish this. Extrude boss involves giving your sketch Depth in the 3D model. Now to do this select your sketch and highlight it. Then by either going to the Features-->boss--> and then to extrude or by selecting Extrude boss option in the right hand side toolbox. Now by selecting this function, you should get extrude boss window menu which looks like this:

Extruding boss will work based on the sketch that you have selected. The direction of the extrude should be set at along normal unless the designer would like to select the direction. This option will require an axis which has been inserted by the user previously to this step. Also the axis which is inserted must be in the correct orientation to the sketch (perpendicular) to the sketch. The draft angle will determine angle from the original sketch to the projected extruding of the sketch. This option can be done normally or outwards which will reverse the draft angle of which the sketch is extruded. Examples of this is show simply in the following images:

Now the type of which the extrude bossing can occur is change able at the type tab in the extrude boss window. To depth will change the extrude bossing based on the specified depth entered at the depth field. This can be reversed depending on the needs of the designer for the model. The Distance can also be done manually as well in the drawing area in which there should be an arrow point towards the direction which was set by the user. By left clicking and dragging the arrow will change the distance of the depth which is added.

Another option which is available for the types of extrude bossing is "To mid-plane". This option will use the plane of which the sketch is based on and project the depth of 3D model on the front and the back of the sketch specified by the user set in the depth field. By selecting in the type field "to Next" will require you to nearest face of that orientation. This will not work if the sketch is not within in reach of the next 3D model. Therefore the model must be within the same boundaries as the sketch in which is being extruded to. By choosing the option to the Next geometry, this option will be based on the next axis or the plane that has been inserted previously and the model itself will be extruded to that orientation. With Each of these options you can rename the Model or the feature itself by filling out the Label Field which will then be placed within the design explorer.

Extrude Cut is putting an cut-out within the 3D model which can only be done if there is an existing 3D model. The Options for the extrude cut are identical to the extrude boss. The only difference is the function of the extrude.

Revolve boss and cut

  Revolve bossing and cutting are different from the extrude boss and cut in a few key areas. The revolve boss will require a sketch with a reference axis or edge for the function to work, where as the extrude only needs a set direction and a sketch. Cutting is also within the same principle as the bossing in the sense that they both require a reference line or an axis to revolve around. The fields are also different since that the dimensions of the revolve is based on the distance between the sketch and the axis as well as the size of the sketch.

To do a revolve boss or cut, these opinions can be selected in a similar fashion as the extrude boss or cut. By selecting the Revolve boss or cut through the right hand side tool bar or through the features menu select either boss or cut and then selecting revolve, will open up a new revolve menu which will allow you to do the following: Selecting the Sketch that is to be used function, the angle in which the sketch is meant to revolve to, the axis in which the sketch is meant to follow in the revolution as well as the name of the feature. Take note that the Axis will not work if selected other than the axis which the plane that the sketch is on. For example if the sketch is on plane ZX, there for the only axis which will work in revolve cut or boss will be Z or X not Y

Now for the Revolve cut to work is that an existing 3D must be present within the drawing area of it. the revolve cut must not also be integrated with the previous sketch or that the 3D revolve cut will fail.

Loft Boss and Loft Cut

  The loft bossing requires two things before the model can take shape. The first requirement is that there must be two sketches for the Lofting to work. The second is that one of the two sketch must be on a different plane that must be parallel to the first one as shown here:

With loft bossing, you can access the option at the right hand toolbar or the feature menu on the top of the screen. After selecting the function you will get a menu, with various fields which you can enter values to help shape the loft boss that you are designing. Now to enter in the cross sections, you will need to highlight the selected the two sketch that you would like to loft boss and then double clicking on them to enter them into the field (make sure you do one sketch at a time and keep the loft boss menu open). Now there are opinions where you can specify the tangent magnitude or the angle for the loft to take. Normally this is turned off if you are using Guide curves. There are three options in using guided curves:

Global Guide curves creates virtual guide curves in turn affect any other guide curve which is using loft surfaces to be affected.

Local Guide curves are isolated to the the loft that is be created.

Tangent Guided Curves are affected by the Loft surface to follow the tangent vector of the guide curve at the point where the curve intersects. 

As before with all the other cutting methods normally used, the requirement of having an existing model is required before the loft cutting can be done.

Sweep Boss and Sweep Cut

  Sweep cutting or bossing will require to have a sketch of the shape desired as well as the direction and distance of the sweep. With Sweep bossing or cutting, you can access the option at the right hand toolbar or the feature menu on the top of the screen. After selecting the opinion, you will be able to get an another window to open up which will give you various fields to enter before the sweep cut or bossing is done.

Firstly, the first field will allow you to choose the sketch in which is to take shape through the sweep bossing or cutting. The Next field under that will allow for the path in which the sketch is meant to either extrude in a sweeping fashion or cut in a sweeping fashion depending on the function selection. Return back to the top of the menu window for the sweep boss or sweep cut, there is a field for the type of sweep. Two options are available to choose from : Through Entire Path is the generic selection which no specification besides the path which it is given. To geometry will give the option of placing a geometry specified by the user to follow along that geometry using the same path. If the type of sweeping is chosen to "To geometry", there are geometry target field as well as the geometry offset available as well. The next field the Draft angle which is the same function within all the 3D modelling in Alibre. Lastly the final field will allow for the user to add a name to the sweep cut or the sweep boss. Here are some examples of what the sweep Cut and sweet boss looks like:

Helical Boss and Cutting

  With helical bossing or cutting it is important that majority of the helical shape is based on the reference lines which are put in placed by the user and then how much of pitch, height or revolutions is forced upon the model itself. An important note to remember with doing anything with helical bossing or cutting is try to limit the amount of helixes required for a model due to the fact of these models are usually very resource demanding on the computer system. One more point to remember with helical bossing and cutting is that the orientation as well as the reference line play major Key factors when forming the the helical boss or cut, so if any problems occur please check that these are in place at the right positions and in the right orientations ( models with multiple reference lines need to be aware of this).

To start off, we will be start with designing a helical boss. To do this you need to choose a  working plane to work with and start by drawing the circle cross section or what every sketch you intend to be the cross section to be in your design. Now using the dimensions tool click on the vertical axis on your working plane (e.g -Y axis on a XY plane) and then to the edge of the cross section and set a distance for the radius of your model to revolve around. Once you have done that make sure you add dimensions to your cross section as well. After that is completed, you will notice a reference line on top of the axis itself. This is the reference line which will be used in making your helical boss. By clicking on the helical boss tool in the right hand toolbar or going to Feature--> Boss --> Helix, will open another window which will allow for the helical boss window to appear like shown the example here:

Now the sketch as well as the reference line should be automatically placed, but make sure it is the correct reference line that you want your model to revolve around. Next you may select one of the two options of making the model revolve around clockwise or anti-clockwise as well as making the model boss in the opposite direction to the the initial projected path shown by the grey line.

The type of the helical bossing can be selected here based on the needs of the designer. Height and pitch will give you the opinion of choosing the height of the helical boss required and then the pitch in which the cross section is revolve around. The pitch type can also be selected here as well as either a constant pitch, variable ratio or variable end. Specification of the model design can also be entered here as well. The height and revolution will allow you to specify the required height as well as the amount of revolutions around the cross section is revolve around the reference line. Revolution and Pitch is a combination of the two since that with the previous fields you are able to enter the height and now want to edit the revolutions and the pitch specifications for the model. Finally the last type which can selected is spiral. As its name suggest it will create a spiral and allow the use to determine the amount of revolutions as well as the pitch. Note that the height field is the radius of the spiral which can be entered previously to any of the other types before hand. The Taper of the model and the name can also be entered here in the helical boss window as well. Click OK to generate the model.

You may have noticed in the helical boss window that there is another tab called advance. This tab will allow you access additional options such as determining the starting conditions as well as the end conditions of the model designed in helical boss here. The profile orientation can also be determined based on being parallel to the reference line or normal which is based the user previous selection in the main tab.

Helical Cut is process which will require first of all a 3D model to work on for the helical cut. Now for the helical cut to work, you need to make sure that the geometries you are using a spot on to what you want the cut to start at. Firstly by using a cylinder to design a thread, we create this by drawing a sketch of circle and then extruding the model to the desired length. Now to design the cross- section which will cut the model in a helical fashion, we will focus the model to the end of the shape where the helical cut is to start. Next select the plane to work on and sketch the cross section like so with the necessary constraints. Make sure that the cross section is at the correct position to the 3D model and to do this, you can use the intersection constraint tool. Next using the reference line tool, create a reference line for the cut to revolve around the model. Once completed, click on the helical cut tool and enter the correct sketch and reference line into the fields required. Select the necessary type, pitch height and revolution and Naming the model. Once completed, Click OK and helical cut will be completed. Here are some images of key steps in process of helical cutting.

Shelling

  Shelling is very straightforward process of selecting a face and limiting the thickness of the sides for the model to be "shelled" out or to remove everything through the model based on the face which was selected by the user. To do this, ensure that you have a 3D model to work with and then by selecting a face then shell on the right toolbar. You can select shell as well through the features toolbar on top. A shelling window will appear giving you the option to remove the necessary face in a set direction and also allow you to change the thickness of the shelling process as well.

3D filleting and Edge Chamfer

  3D filleting and Edge chamfer is very similar to the 2D equivalent in Alibre design. 3D filleting will create a rounded edge in which is given by the user to do where as 3D edge chamfer will remove edges and replace it with a flat surface. With both of these functions, they can be selected through the right hand toolbar and select the fillet icon or you can right click on the model and select either the edge chamfer or the fillet option there. Once the window for 3D fillet or edge chamfer appears select the required surfaces to perform the function and set the specifications for the distance of the fillet or the edge chamfer required to completed. Click OK to complete the process and the model will generate the edge chamfer or fillet required.

Holes

  As the name suggest, this function will allow the creation of holes to your Alibre design model. To activate the function simple click on the hole icon on the right hand toolbar or using the feature menu on the top toolbar and select the hole option. This will open a hole window with a list of field which you can enter the specification as well as label and select the required type of hole need to be made in the model as shown here.

Once you have completed entering the required fields as well as details for the hole, click OK to generate the hole in the model. Now sometimes you will need to design more than one hole in the model, the pattern tool will help  to accomplish this in the next heading.

Patterns (linear and circular feature)

  The pattern tool is available to Alibre designer to generate models which require more than one feature to be placed on a model in a linear or circular fashion. The pattern tool can select a feature and repeat that feature in a linear or circular fashion to save time for the user. To activate the linear Feature pattern, select the linear pattern icon in the right-hand toolbar and a linear feature pattern window should appear like the following image shown.

Now select the feature required for the pattern replicate and then enter in the spacing between the feature as well as the number of copies which are need. Next select the linear path on the model itself to tell the pattern to continue in what direction and then select the second linear path if required to repeat the pattern. Once completed, you can change the label name of your pattern Feature and click OK once you are happy with pattern to reproduce.

With the circular pattern, this function will only create holes around a reference line or a selected vertex as a centre where the pattern will be placed in a circular fashion. To activate the circular feature pattern, select the circular pattern icon in the right-hand toolbar and a circular feature pattern window should appear like the following image shown.

Now just like the linear feature pattern, select the feature required to be repeated and then select the reference line in which the pattern is to rotate around. Next choose the amount of copies which are required for the pattern to complete and also the angle in which the pattern is to repeated as the pattern is revolved.

Boolean Feature

  Boolean Feature in Alibre will help you subtract and add to other Solids which are used in the 3D as well as show the overlap of the models used. Now with Boolean Feature to work firstly you will need two solids models to work with. One of the two models is known as the Tool. This is termed used any part or assembly which has been created or save. Now the other model which will be designed in the work space is known as a Blank. This refers to a basic 3D model which used to join the Tool onto usually in mould making. To add within Boolean Feature Firstly design the 3d model or open an existing project in which you like to use to either add or subtract from. Next select the Boolean Feature icon (choosing the correct icon for subtracting or adding) on the right hand toolbar and select the Tool in which would like to use. The feature will display a different workplace to use and also the model in which you are importing click once to place your model in the workplace and then finish to complete the task. The workplace display now should be the similar layout as the image shown here. This workplace is known as the Design Boolean Workplace.

Now to manipulate the tool which has been placed. select either the face or the planes in which the model is best to be edited from and then select the insert assembly constraint tool. It will give you window in which can edit the orientation, align or mate the tool. There are two other functions which are also can be used. these are the angle as well the tangent constrains. These are readily available for the user to choose how they want to orientate the tool place in. Once completed with the constraints to return and accept the changes within the boolean model.

Inserting Catalogue Features

  Within Alibre Design, you can add and insert features to your model design from a catalogue which you have maybe created previously. A catalogue is a a list of features in Alibre design which have been saved previously, so it can be used again in other models. To save features within the model simple go to feature tab on the top of the toolbar and then save catalogue feature. A window should open with a field required for you to highlight the feature you want to save. Click on the field to activate and then select the feature from the design explorer. Next click save as and store it to a folder which you would like.

To insert the feature, go to the insert catalogue feature on the right hand toolbar and then find the feature through the browse button. Once you have found the feature, select and then click Ok. Then you will return back to the previous window for inserting catalogue features and you can select the face in which the catalogue feature is to be placed. Now you can align the feature to a plane or reference point by selecting the plane or reference line in the align field box. To finish simply click apply.