Belts/Chains

[Rion Atkinson]

I have been trying to create chains for the past two hours. I am able to create the layout of it using the belt/chain tool. But I am unable to get either a belt or a chain to actually show up. Does anyone know how to do this?

Thank you.
-Rion

[mplanchard]

In SolidWorks, To create a belt/chain assembly feature:
1. Click Belt/Chain (Assembly toolbar) or Insert, Assembly Feature, Belt/Chain.
2. Set the PropertyManager options.
3. Click OK .
In the FeatureManager design tree, the following appear:
• A Belt feature. The belt length appears next to the feature.
• A BeltMates folder (under Mates ), containing mates between adjacent pulleys.
To see the belt curve when the PropertyManager is closed, select the Belt feature in the FeatureManager design tree.
If you selected Create belt part, a new part containing the belt sketch is created and added to the Belt folder in the assembly. The part has:
• An external reference to the assembly.
• A LockToSketchMate that constrains the belt part to the belt sketch.
• Custom properties Belt Length and Belt Thickness.
If you selected Engage belt, you can drag to rotate one pulley to see all the pulleys rotate.
If you did not select Engage belt, you can reposition one pulley without causing the others to rotate.
Marie

[Rion Atkinson]

Originally Posted by mplanchard

In SolidWorks, To create a belt/chain assembly feature:
1. Click Belt/Chain (Assembly toolbar) or Insert, Assembly Feature, Belt/Chain.
2. Set the PropertyManager options.
3. Click OK .
In the FeatureManager design tree, the following appear:
• A Belt feature. The belt length appears next to the feature.
• A BeltMates folder (under Mates ), containing mates between adjacent pulleys.
To see the belt curve when the PropertyManager is closed, select the Belt feature in the FeatureManager design tree.
If you selected Create belt part, a new part containing the belt sketch is created and added to the Belt folder in the assembly. The part has:
• An external reference to the assembly.
• A LockToSketchMate that constrains the belt part to the belt sketch.
• Custom properties Belt Length and Belt Thickness.
If you selected Engage belt, you can drag to rotate one pulley to see all the pulleys rotate.
If you did not select Engage belt, you can reposition one pulley without causing the others to rotate.
Marie

I am able to get the belt to work, such as being engaged and such. But no matter what I try, I can not get a physical model to show. Do I have to create this on my own? Or is there a tool that will automatically create a physical model of #35 chain, or even a belt, on the same path as the belt on the CAD drawing?

[mplanchard]

Once you create your belt sketch and calculate the length in SolidWorks, then you have to develop the belt as a part in the assembly. Save your assembly. From within the Assembly,
1. Click Insert Component, New Part.
2.Select a plane (usually the plane of your belt sketch). The FeatureManager inserts a new part and is displayed in blue.
3. Hold the Ctrl key down and select the belt sketch (or right click select chain)
4. Click Convert Entities. Click Extrude Base. Enter your belt depth and direction.
If you need cuts in your belt:
1. Click the face of the belt. Click Sketch. Click the inside belt tangent edges. Click Convert Entities. Exit the Sketch you will need this for your pattern.
2. Create an Extruded Cut.
3. Click Pattern, Curve Driven Pattern, Select the belt and select convented sketch. Enter number of cuts. The pattern will follow the tangent curve.

The same procedure is for a chain. You need the sketch of the belt from the assembly. Copy this to a new part and create one individual link. Pattern and Mirror save rebuild time.
See http://www.3dcontentcentral.com/secu...d=171&id=10717 Marie