Surface toolbar

Surfaces toolbar comprises of tools like Extrude, Revolve, Sphere, Cylinder, Offset, Sweep, Fill, Offset, Blend etc. You can see all of the tools present in the attached picture. There are a few differences with regards to the sketch as we used it in the part-design workbench. 

Surfaces toolbar

If you remember, in the part-design workbench we read about the conditions that need to be met for a valid sketch. You can read about them here again if you have forgotten. Nonetheless, the condition i.e. sketch should not be open does not apply in surfacing and you can use a closed as well as open sketch for making a surface.

Extrude

You can use a plane for making a sketch, as you did in the sketcher and part-design workbench. After you have made a sketch you can extrude it using the extrude command. Below, you can see a rectangle has been extruded. As you studied in Part design with Pad command, here too, you can apply mirror extent or extrude the sketch independently using different lengths. 

Surface created by extrude using a rectangular sketch

You can also specify alternative directions and extend the sketch upto any particular element if you like. So in many ways it is similar to the Pad command in Part-Design. However, the result it produces is different since it creates a surface of zero thickness.

Revolve

The revolve tool is much like Shaft in Part design workbench, except that in this case a surface is created instead of solid. You can use any kind of sketch you wish, and by default axis made in the sketch will be used for rotation. You can also use any line or any other axis too for rotation. 

Revolve used to create surface

A thing to keep in mind is that the sketch cannot be self-intersecting. Not only can you use the sketch for rotation, you can also use the wireframe line / points for revolve and can create geometry. 

Sphere

Spherical surface can be made easily with the use of this tool. Not only can you make complete sphere, but also parts of sphere by specifying meridian end angle, start angle and other parameters. By default the sphere will be in the default axis system. 

Spherical surface made using Sphere tool

If you are working with different axis systems at once, you can use an axis system for reference and it will orient the sphere with that as reference.  

Cylinder

To create a cylindrical surface, you would need to define a point about which you wish to create a cylinder. In addition you would need to define a line about which the axis needs to be oriented. The orientation can also be about X, Y or Z axis.

Cylinder surface created about origin

Other parameters that you can set to define the cylinder are lengths in two direction and radius of the cylinder.

Offset

Offset command can be used to copy and offset surfaces as we prefer. Even the most complex surface can be offset and copied using this command. If needed, you can offset the surface on both sides i.e. a copy will be created on either side at the same distance that you specify.

Offset used to create two surfaces

To create more than one copy, you can use the option, 'Repeat object after OK' this will ask for number of copies that you wish to create and will create the required copies. A local smoothing is applied only if the constant offset cannot be performed, you can use automatic or manual options to define this. It would clean the geometry of the surface and enable the offset. In case you are facing problems with the offset, you can use the tab 'Sub-elements to remove' and select the surfaces which may be creating the problem and remove those particular surfaces.

Sweep

Sweep is perhaps one of the most difficult option to understand and use since it involves so many options. The option has four major sub-options based on profile type and these are:

1. Explicit
2. Line
3. Circle
4. Conic

1. Explicit - Explicit option itself has several sub options. However, what's worth remembering is the fact that it requires an profile to be specified i.e. you will need to provide a sketch or a profile that you wish to sweep using guide curve or other sub options that are available like, with reference surface, with two guide curves and with pulling direction. Let us see these one by one.

With reference surface 

The option will sweep the profile along the guide curve. The reference surface will be mean plane of the guide curve you select. If needed, you can select the surface (you need to be careful that you select the surface on which the guide curve lies) and with the help of this, you would be able to exercise Law option and rotate the profile about the guide curve. 

Explicit profile option used to create a surface using the sub-type i.e. Reference surface

You can use relimiter1 and relimiter2 to limit the surface as per requirements. To have predictable results, it's best to select spine as the same as guide curve. A plane was used a Relimiter 1 while ZX plane was used as reference surface and profile was rotated by 19 degrees. Both profile and guide curve are in thick orange colour. The best way to utilize this option is to as you would use Rib in Part design workbench. I would suggest you to try it out on your own and get the feel of this tool.

Another surface created using Explicit profile - with reference surface

Above you can see another example, the profile can be seen in green colour and guide curve in blue and surface in yellow. The surface is created exactly at the location where the profile is positioned with respect to the guid curve.

Section of the rotated surface shown, created using Sweep - Explicit profile with reference surface

If needed, the surface can be rotated about the guide curve with use of appropriate reference plane i.e. the plane in which the guide curve lies. Above you can see the surface rotated and section of the surface is shown to depict how it has rotated with respect to the profile.

With two guide curves 

Consider it as an extension of the option 'With reference surface', considering you get the option to specify two guide curves. The difference is that there's no reference surface that you specify, so there's no way to manipulate the profile about the guide curve. Other options like relimiters etc. are the same. A thing to keep in mind with regard to this option is that you need to take care of the guide curves. The anchor points are computed automatically, however, if you use the start points of the guide curves as starting points, it gives predictable results.

Surface created using Explicit profile option - with two guide curves

You can see the profile used for creating the surface in the purple color while guide curves are in green. The two anchor points have been selected explicitly as it creates the desired surface.

With pulling direction

The option is similar to the option that was present in Rib as well as Slot in the Part design workbench. So, when you use a direction as pulling direction for creating the surface, the profile will be dragged along the guide curve. 

Swept surface created using pulling direction. Profile in blue and guide / spine in green

A thing to keep in mind is that to have predictable results, you should use the option 'Projection of the guide curve as spine'. The pulling direction chosen results the profile to maintain the same angle with that direction. If you use the same profile and guide in case of Rib and slot with the option 'with pulling direction', you will get a solid that has same outer surface as that of this one. 

2. Line - This option relies on making surface with the use of line or lines. If you compare it with the Explicit profile option, there's no profile required to be made in this case. The option has many sub-options like two limits, limit and middle, with reference surface, with tangency surface etc. Let's see how they work.

Two limits and  Limit and middle

Two guide curves can be used for making a surface. These guides act as limits where the surface ends. However, the surface can be extended using the option of Length 1 and Length 2. 

Surface created using line profile, two lines as guides

The surface in this case is extended by 20mm in one direction using the Length 1. The surface can be re-limited too using planes using options Relimiter 1 and Relimiter 2.

Limit and middle

This is just another option and can be used from within the Two limits options. You can exercise this using the option "Second curve as middle curve" from within as can be seen above. It will extend the surface equally on both sides of the second curve.

Surface made using the line type profile and Limit and middle as option

So in essence, you are defining the middle curve about which there is limit at one end defined by one guide and on the other end surface extends by equal distance. 

With reference surface

The options is perhaps the best tool to create surfaces with curves lying on surfaces. The curves lying on the surface may be created by projecting curves or edges on the surface, or simply the edges of an existing surface may be utilized to create such surfaces.

Surface created using line profile with the option reference surface

The flexibility that it offers is that the surface created can be extended using lengths Length 1 and Length 2. In addition, the surface created can be rotated about the guide curve using angle parameter.

With reference curve

The option can be used to create surface using a reference curve inspired from guide curve. The guide curve is essentially the form that is imposed on the reference curve. Angle can be imposed on the created surface and rotated about reference.

Surface created using reference curve and guide curve

Also, the surface can be extended in both directions using Length 1 and Length 2. In the case above you can see that equal length of 20mm is applied and surface is rotated by an angle of 27 degrees.

With tangency surface

A very versatile option and can be used to create surfaces tangential to other surfaces using a curve. It's important to know that the solution should exist, otherwise an error will be shown. It's possible that there may be more than one solution, in that case, all solutions will be shown.

Surface created using Sweep with profile option (with tangency surface)

You can switch the preferred option (shown in blue) using 'next' button. Here you can see that a circle was used to create a tangent surface on an egg shape. You have inbuilt option to 'Trim with tangency surface' which you can exercise to trim the base surface with respect to the new surface.

With draft direction

The option can be used to create surfaces that are almost ready for production and have drafts applied so that it may not be a problem in production. A surface can be created with the use of a guide curve and draft direction.

Surface created using sweep command

Length type i.e. Length type 1 and Length type 2 etc. may be defined using normal method, curve, plane etc. (options shown in green). In this particular case, length of 10mm and 20mm has been used and draft angle of 41 degrees has been applied.

With two tangency surfaces

The option can be used to make a surface that is simultaneously tangent to two surfaces. In addition to specifying two surfaces, you would also need to specify the spine, this can be chosen depending upon the requirement of the surface. Generally it can be the centre curve of any of the surface.

Surface created with sweep using profile option using two tangency surfaces option

Here you can see the options yields four results and you can choose the one you prefer. The one that's selected is shown in orange while others in blue.

3. Circle - The circle profile options makes surfaces that relies on various methods for generating circular surfaces. The circular profile is not used explicitly as in case of the Explicit profile option where you make the profile that you wish to sweep. In this case however, elementary geometry options that you may have studied in school are used like centre radius, two guides and radius, centre and two angles etc. Let us see how 

Three guides

Having three guides is essentially like defining three points varying along a spine through which the surface is generated. so as long as you have one guide that's not co-planar with the other two, the surface shall be generated.

Surface created using Sweep with circular profile option - Three guides

Here you can see that two of the guides are in one plane while the third is in another plane. The surface section created can simply be switched using the guides, the ones you want as limits are selected as first and third. If you want, you can relimit the surface using relimiters 1 and 2.

Two guides and radius

A surface can also be created using two guides and specifying the radius of the circular surface that you wish to create. It's likely that more than one result will be provided. To create the surface in orange, press OK, to switch selection press 'Next'.

Creating a surface using circle profile with the option - two guides and radius

In this particular case, a total of six solutions were offered, as can be seen. If you need multiple surfaces, you can reuse the tool to create as many surface of choice.

Centre and two angles

The option is similar to the two guides and radius. However, in this case the two guides are centre curve and reference curve. In addition to this, you can specify angles if you only part portion of surface, or specify it as 360 if you wish to make complete surface.

Surface created using sweep with circle profile and the option - centre and two angles

The option can also be used to create circular surface pipe around the center curve if you use the option 'Use fixed radius' as we have done. 

Centre and radius

There are many ways to skin a cat as I have repeatedly said, the kind of surface we made using an option within the option Centre and two angles can be exercised directly using Centre and radius. In this case, you need to just specify a centre curve and radius value to make a surface.

Surface created using sweep with circle profile and option - centre and radius

The option is best utilized to make pipe like surfaces, which can be around 2D or even 3D curves. The flexibility that is present in other tools is present here too. Like you can use law to vary radius value at start and end and make surface like above. In the case above, instead of using constant variation, the radius value varies and changes from 2mm to 12mm using S-type law.

 

Two guides and tangency surface

The option requires a limit curve with tangency (lying on the surface), tangency surface and a limit curve from which the surface stretches to the existing surface. The limit curve need not be on the surface as is the case here, but can also be an edge of the surface.

Surface created using sweep with Circle profile with the option - two guides and tangency surface

The result in this case are two surfaces, you can choose the one you prefer. The tool can be use to create surface continuity and join other surfaces. 

One guide and tangency surface

If a guide does not exist on a surface but still you wish to connect it with another curve or surface, you can perhaps use this tool. So, you need to specify one guide curve, this can be a edge of another surface or a curve on another surface, and in addition a surface to which the new surface will be tangent to.

Surface created with Sweep tool and circle profile, the sub option used is one guide and tangency surface

In this particular case, you can see there are four results options. If the surface is not circular (as is the case here) you would also be able to use the option to trim the surface with respect to the newly created surface.

Limit curve and tangency surface

The option can be used to make a new surface from an existing surface and a curve on surface. The curve on surface is the limit curve, while the surface is tangency surface. In addition, you need to specify the radius of the surface that you wish to create.

In this particular case, there are two solutions and we keep the one in orange. Not only can you select a surface of your choice, you can also specify an angle to enlarge / reduce the surface size.

4. Conic - With use of the Conic profile, you can join surfaces or create surfaces from scratch using guides curves and tangency surfaces. It's important to keep in mind that surfaces created will be conic in shape. The options that are available are two guide curves, three guide curves, four guide curve and five guide curves.

Two guides

Two guides with two tangency surfaces can be used to connect two surfaces using this method. The tangency surface that you specify is not optional and you cannot make a surface without specifying it. In addition to specifying the tangency surface, you can specify the angle that the surface maintains with the guiding curve (which by default is zero i.e. surface by default is tangent to the tangency surfaces specified)

Swept surface created using conic profile with use of two guides option

Like here you can see that the angle has not been changed and is zero so it maintains tangency. The parameter value is the same that you entered while making conic during sketcher. So, this parameter value can be between 0 and 1, and it will determine the sharpness of the surface. 

Three guide curves

A conic surface with three guide curves requires two tangency surfaces along with end guide curves and a middle guide curve. It must be noted that the surface will be created only if it conic in cross-section along the spine.

Swept surface with conic profile and use of the option - three guides

Here you can see a surface created with two surface edges used as guides and curve in the middle used as another guide. The newly created surface is tangential to the existing surfaces and passes through the middle guide curve.

Four guide curves   

You can also make a conic surface with the use of four guide curves, it requires one guide curve along with a corresponding surface to which the surface will be tangent and other three guide curves.

Swept surface with conic profile and four guide curves

A thing to be kept in mind is that same conditions like some that we adhered to while making conic in sketcher also applies here. The two pair of lines at least need to be in the same plane to successfully execute this command.  

Five guide curves

With five guides, you can create a conic surface. In this case, you need not specify a tangency surface. However, the guides should be such that they can make a conic surface. Such a surface may be required in a really special circumstance. Nonetheless you should know that such an option exists.

Swept conic profile with five guide curves

Here the each of the two guide are in a plane, while other two in another plane, the fifth in a centre plane. 

Fill

Fill option is very versatile and can be used to create a surface anywhere the boundaries are close. It can either be a boundary comprised of several edge / curves or can be a single curve / edge. However, this will not work if the boundary is not closed.

Top surface created using Fill

Whenever the boundary is closed and a surface can be created, you will be shown the message 'Closed contour'. In this case, after selecting the curve, the corresponding surface (Sweep.1) was also selected to define tangency continuity. It is not essential to define a support, however in that case the surface will maintain point continuity with the surface.

Multi-sections surface

We created Multi-sections surface in the Part design work bench, you can read about it here. The Multi-section surface is exactly the same, however the only difference is that you can use an open sketch as one of the section for making surface while in the part, all sections had a requirement of being closed profiles.

Surface created using Multi-sections surface

All other options such as guide curves, spine, coupling, re-limitations etc. are all the same.

Blend

Blend operation can be used to connect two surface or two curves / edges. The edges or curves used can also specify support surfaces. When these support surfaces are specified, we can specify the kind of continuity of the surface using point, tangent or curvature continuity. 

Blend surface (in yellow) created between green and blue surfaces

In addition to the continuity options, you specify the tension value using the tension tab. Blend has similar options to the multi-sections surface tool and you have coupling / spine and closing points options. All these options work exactly the same as you used them previously.