do you just need to "see" a texture (easy), or do you really need the texture in the 3D geometry (hard)?
Texture in 3D sir. Something like dipples you would see on a golf ball but the dipples must be parallal with the surface and follow the slope of the loft. I see it done all the time but I have never done this before.
Thank you for your time and help
This is difficult for SolidWorks to compute, sometimes impossible.
The only good solution is to use a feature pattern, and try and pattern bodies. Fill pattern and 3D Sketch Pattern both can accomplish what you are looking for, especially if you want to pattern little spheres (either embossed or debossed). Other shapes are much more difficult or impossible.
Can you tell me more about fill pattern?
Fill Pattern is great for this type of thing, but only on flat surfaces. Since yours is curved, you need to use a sketch driven pattern, using a 3D sketch as your Reference sketch (see my following post)
The Fill Pattern feature lets you select an area defined by co-planar faces or a sketch that lies on co-planar faces. The command fills the defined region with a pattern of features or a predefined cut shape.If you use a sketch for the boundary, you may need to select the pattern direction.
Parameters control the pattern layout. You can create a sheet metal perforation-style pattern, or a pattern of concentric shapes typically used to enhance aesthetics.Typical uses include:
- Weight reduction
- Ventilation holes
- Grip surfaces
Types of Fill Patterns
Predefined Cut Shapes
If you select a vertex, the shape seed feature is located at the vertex. Otherwise, the seed feature is located at the center of the fill boundary.
Diamond cut shape. Square pattern using 4 instances per side. No vertex selected. Same parameters except vertex is selected.
- Fill Pattern PropertyManager
The Fill Pattern PropertyManager appears when you create a fill pattern.
Sketch Driven Patterns
Using sketch points within a sketch, you can specify a feature pattern. The seed feature propagates throughout the pattern to each point in the sketch. You can use sketch driven patterns for holes or other feature instances.
To build a sketch driven pattern:
- Open a sketch on the face of a part.
- Create a seed feature on the model.
- Click Point or Tools > Sketch Entity > Point, and add multiple sketch points to represent the pattern you want to create, based on the seed feature.
- Close the sketch.
- Click Sketch Driven Pattern (Features toolbar) or Insert > Pattern/Mirror > Sketch Driven Pattern.
- Under Selections, do the following:
- If necessary, use the flyout FeatureManager design tree to select a Reference Sketch to use as the pattern.
- Click either Centroid to use the centroid of the seed feature, or Selected point to use another point as the reference point.
Depending on what you select as your Reference point, the position of the features you propagate will change. Origin used as the Reference point Selected Vertex used as the Reference pointYou can also alter the relative position of the features you propagate when using a table driven pattern.
- If you chose Selected point as the reference point, select a Reference Vertex in the graphics area.
- You can use the centroid of the seed feature, the sketch origin, a vertex, or another sketch point as a reference point in a sketch driven pattern.
- Do one of the following:
- To create the pattern based on the feature, under Features to Pattern , select the feature in the graphics area.
- If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features.
- To create the pattern based on the faces that make up the feature, under Faces to Pattern , select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself.
- When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries . For example, a cut across the
- entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
- To create a pattern based on multibody parts, under Bodies to Pattern , select the body to pattern in the graphics area.
- Under Options, set these options:
Geometry pattern Creates the pattern using only the geometry (faces and edges) of the features, rather than patterning and solving each instance of the features. The Geometry Pattern option speeds up the creation and rebuilding of the pattern. You cannot create geometry patterns of features that have faces merged with the rest of the part.
Geometry pattern is not available with Bodies to Pattern.
Propagate Visual Properties Propagates SolidWorks colors, textures, and cosmetic thread data to all pattern instances.
- Click .
Ok I have looked into using those but dont they only work for flat surfaces?
Ok well I didnt know I could do that, but once I get the shape I want I do I have it follow a loft? I would like to do a cut in the surface and keep all cuts at the same depth along the loft. Is that possible?
Thank you Mr. Marsman
See below and attached. I have modified your model with how to apply this as a sketch pattern.
1911_grips_blank_right_cc.SLDPRT.zip 282.7 KB
You Sir are the Awesome!!! I got it to work on my part which is a slight bit different then the one I uploaded but it worked!! Thank you
My name is Carl and thank you everyone for your input and help.
Trying to do this with something other than spheres is where SolidWorks has difficulty. There is no way to set the "normal direction" of the feature, so it cannot "follow" the curvy surface. It will simply pattern itself in the exact orientation that the first feature is. So with a sphere that does not matter, but with any other shape, this will be a problem. There is no way to do this perfectly with other shapes.