What is Loft Tool in SolidWorks?

The Loft tool in Solidworks is used to create a solid or surface between multiple profiles. It produces high-quality and accurate surfaces that can be used for creating complex and organic shapes for product design. Its usage ranges from the aerospace, automobile, and shipbuilding industry to making normal day-to-day home appliances. However, this tool is overshadowed by the Boundary tool, which allows more accurate control over the shape. But the Loft tool does provide some features that the Boundary tool lacks such as the use of centerlines, or the creation of closed-loop lofts, and it also allows you to add sections to the loft shape.

SolidWorks provides 3 ways of using the loft tool:

1. Lofted Boss/Base: It is used to create a solid lofted body. Click on the Lofted Boss/Base tool in the Features toolbar or go to Insert -> Boss/Base -> Loft.

2. Lofted Cut: It is used to remove solid material using the lofted body. Click on the Lofted Cut tool present in the Features toolbar or go to Insert -> Cut > Loft.

3. Lofted Surface: It is used to create a surface lofted body. Select the Lofted Surface tool present in the Surfaces toolbar or go to Insert -> Surface -> Loft.

While creating loft profiles keep these things in mind:

• The Loft tool requires at least 2 profiles if you want to create an open loft while 3 profiles are required to make a closed loft.
• The profile cannot contain multiple contours (open or closed) unless you know how to use the Selection Manager. You can use just a point as the profile, but you can do it only for the first and last profiles. Intermediate sketch profiles must contain open/closed entities.
• If you want to create a solid loft, all profiles must be closed. But for a surface loft, you can use open profiles.

What are the Connectors in Loft tools?

A connector is a polyline that interconnects profile vertices. Connectors are added at the end point of every segment of the profile sketch automatically by SolidWorks. You can manipulate these connectors to help you obtain the shape that you want, by allowing you to adjust how the sketch segments of profiles are connected to each other to create the Loft feature.

Tip: Most beginners usually think that connectors added by SolidWorks are random. But that’s not the case. SolidWorks places the main connector at the nearest vertex point where you click to select the profile. Take a look at how the green connector changes its position as we use a different line of the sketch to select the profile.

Usually, only one, the main connector is visible. If you want to view all the connectors, right-click on an empty area and select Show All Connectors. You can hide all the connectors by clicking on the Hide All Connectors button.

You can notice that even when the connectors were hidden, you can see where the connectors actually were as yellow lines. The yellow line in the Loft preview actually depicts the edges of the loft which generally have connectors.

To edit a connector, drag any of the handles . If you mistakenly moved any connector, right-click on an empty area and select Undo Connector Edit. Use the Reset Connectors button if you want to reset all the connectors to their original position.

You may notice that there are 2 types of connectors, one with a green handle and one with a blue handle.

• The one with green handles is the main connector as it is the first connector on a profile with non-tangent edges. It can only move from vertex to vertex along an edge. When you drag the handle, it will jump to the next vertex.
• The ones with blue handles are the supporting connectors. You can drag them anywhere along the profile to get the shape you want.

You can always add additional connectors to give you finer controls on the loft shape. To add a connector, right-click an edge on the profile where you want to add a connector and select Add Connector. Once you add connectors to profiles, you can reposition them.

However, since the connectors are made up of lines they don’t allow you to have finer control over the shape. So guide curves are used.

What is Guide Curves in Loft?

Guide curves are sketch entities, any kind of curves, or model edges that are used to define the shape of the loft between the profiles. You can also use Curve Through Reference Points as a guide curve, selecting corresponding vertices of the profiles to create the curve.

You can use Guide Curves along with Connectors or you can make enough guide curves that there will no longer be any connector needed by the Loft. When creating lofts with guide curves you should keep these things in mind in order for the loft feature to be successfully completed.

1. All the guide curves must intersect with all the profiles, even if the profile just consists of a point. But there is no hard rule that the guide curve must end at the first/end profile of the loft. Guide curves can be longer than the resulting loft. But the loft will terminate at the end of the smallest guide curve.
2. You can add as many guide curves as you want. The more the guide curves, the more control you will get over the shape.

Follow the steps given below to make a loft with guide curves:

1. Under the Profiles menu, select all the profiles. You can use sketches, faces, or edges as profiles. The loft will be created in the same order as you select the profiles. Use the Up-Down arrow key to set the order of the profiles if needed.

2. Define Start/End Constraints if and as needed.

3. Under the Guide Curves menu, select all the guide curves. Use Selection Manager if the normal click-to-select does not work as you want. Right-Click in the graphics area and click on the Selection Manager. The Guide Curves Influence Type will be defined in the same order as you select the guide curves. Use the Up-Down arrow key to set the order of the guide curves if needed.

4. Under the Guide Curves menu, you will find the Guide curves influence type. This setting controls how the guide curve is going to influence the shape of the loft. Select one of the following:

• To Next Guide: When selected, the guide curve will only influence the shape of the loft until the next guide curve.
• To Next Sharp: If selected, the guide curve will only influence the shape of the loft until the next sharp of the profile.

Tip: A sharp is a hard corner in the profile. If there is no tangent or equal curvature relation present between any two contiguous sketch entities then that will be defined as a sharp.

• To Next Edge: When selected, the guide curve will only influence the shape of the loft until the next edge.
• Global: When selected, the guide curve will influence the entire loft.

5. Under the Guide Curves input box you will find the Guide tangency type option. This setting allows you to control the tangency where the loft meets the guide curves.

• None: Tangency constraint is not applied i.e. zero curvature.
• Normal to Profile: If selected, this applies a tangency constraint that is normal to the plane of the guide curve. You can then set the draft if required, in the Draft Angle input box. Use the Reverse direction icon present alongside the input box to reverse the direction of the draft.
• Direction Vector: It will allow you to use any entity that you select as a direction vector for applying a tangency. You can select a linear edge or axis, face or plane, or a pair of vertices to set the direction vector. You can then set the draft if and as required.
• Tangency to Face: It makes the lofted surface tangent to the faces that lie along the guide curve. (This option is only available when the guide curve lies on the edge of existing geometry.) Note that the Tangency To Face will result in a loft failure error if one or more profiles have an angle greater than 30 degrees to the tangency faces. The ideal angle is 2 degrees or less.

5. Define other options as per your liking and Click Ok. To get a detailed explanation of each option, go to How to use SolidWorks Lofted Boss?

6. Use options under the Curvature Display menu to check how your loft is propagating. You can select Mesh Preview, Zebra Stripes, or Curvature Combs to better understand the flow of the surface.

How to handle Loft errors?

1. Guide Curve No.1 is invalid. It does not intersect with Section No.1

If you get this error, then make sure that the guide curve intersects with all the profiles. This kind of error message is very easier to fix as it tells you which guide curve is not intersecting with which profile. Sometimes it may look like the guide curve is intersecting when it actually is not. Like in the image below, the spline which will be used as a guide curve has a coincident relation with the circle of the profile sketch. But still, there is a huge gap. So, always make sure that there is a pierce relation present unless you have added a coincident relationship between points.

2. Guide Curve is not selected.

Right-click in the graphics area and choose SelectionManager, then select the guide curve or you can always use the different sketches for individual guide curves.

What to do if the Loft is not propagating the way you want?

• You can control the behavior of the loft by creating the same number of segments on all the guide curves. The endpoints of each segment mark corresponding points for the transition of the profiles. Use mesh preview to get a better understanding of how the loft is propagating between your guide curves.

• You can do the same with the profiles. Creating the same number of segments on all the profiles will make the endpoints of each segment mark corresponding points for the transition between the profiles.

And that’s it. We hope that this article helped you learn how to use the Guide Curves in the Loft tool in SolidWorks. If you have any questions or suggestions, feel free to leave a comment down below.