Creating a Laminated Stock

Steven Kiley

12 Sep, 2021 09:54 PM

In this tutorial, I will show you how to create a laminated wood stock. This is really only useful for creating convincing renderings of laminated wood, but could also serve to illustrate manufacturing intent on a drawing. I will be demonstrating some intermediate to advanced surface modeling techniques and tools. Prior knowledge of regular and 3D sketching is required, as well as creating reference planes.

1. Step 1: Creating Reference Sketches

   • Start on the Front Plane and create this sketch:

   

   

   • Finish the sketch and select the Reference Plane tool.
   • Create the following reference planes:

   

   

   

   

   • Once finished with the planes, create the following sketch on the Front Plane:

   

   • Extrude the sketch as a surface with the following parameters:

   

   • Next, Create the following sketch on the Top Plane:

   

   • Extrude the sketch as a surface with the following parameters:

   

   • Start a 3D sketch and use intersection curve to create lines out of the three surfaces:

   

   • Hide the surfaces for clarity.
   • Start a new sketch on the Right Plane and create this rectangle:
   • NOTE: The rectangle is fully defined with constraints, only requiring a dimension for the fillets. I've shown the sketch against white to see the previous sketch lines easier.

   

   • On Plane 4, create the next rectangle:

   

   • On Plane 3, create the following profile:

   

   • On Plane 2, create the following profile:

   

   • On Plane 1, create the following profile:

   

   • You should now have the overall skeleton of the stock laid out.

   

   Now we will begin to create some surface geometry with our sketches in place...

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

2. Step 2: Lofting our Stock Contour

   With our reference sketches as 'framework', we can begin to loft our profiles together.

   • Activate the "Surface-Loft" tool and select the three highlighted profiles shown below:
   • NOTE: It is important to select the profiles in order from left to right, or right to left. Otherwise the loft will fail.
   • Select the highlighted guide curves shown below:

   

   • Start another "Surface-Loft" and select the following profiles and guide curves:

   

   • Start a new 3D sketch and convert the following lines and edges to sketch entities:

   

   • NOTE: The conversion of the edges is not necessary, but a precautionary step, just in case our next feature fails. We can save these edges for later by simply converting them to construction lines:

   

   • Close out the 3D sketch and open the "Boundary-Surface" tool.
   • NOTE: because we have sketch entities over the edges, we will need to use a selection filter.
   • Enable the "Filter Edges" selection filter and select the two profiles shown below:
   • Turn off the selection filter and select the four 3D sketch segments as 'guide curves'.
   • DO NOT close the command yet. In the blue box, where your profiles are selected, highlight the first one and then change the drop-down box below to "Tangency To Face.
   • Do the same for the second profile, then finish the command.

   

   

   • Once complete, you'll notice that our first three surfaces are not merged. This is normal. Your model should look like this:

   

   • We're now going to use the "Fill Surface" tool on either end of the model.
   • With the "Fill Surface" tool active, select the open rectangular edge.
   • Finish the command.
   • Open the "Fill Surface" tool again, and do the same to the open elliptical edge on the far side.

   

   

   • Now, activate the "Knit Surface" tool and select all five surfaces.
   • Be sure to check "Create solid" and "Merge entities" then finish the command:

   

   • Your model should look like this:

   

   With the surface modeling converted to a solid, we can now add some "machined" features to our stock...

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

3. Step 3: Creating 'Machined' Features

   We are now ready to add the features to our stock that would mechanically fix it to a rifle. The following steps should be fairly basic for the average SolidWorks user. There will be a few more surface features for trimming purposes.

   
   

   
   

   • With Sketch 1 visible, start a sketch on the Front Plane and use 'Convert Entities' on the front edges of the stock.
   • Extrude the sketch (solid) with the following parameters:

   

   • Fillet the following edges with the parameters below:
   • NOTE: Tangent Propagation is unchecked.

   

   • Chamfer the following edges with the parameters below:
   • NOTE: Tangent Propagation is unchecked.

   

   • Create the following slot sketch and cut-extrude it with the parameters below:
   • NOTE: The slot length is measured from the edge highlighted orange.

   

   • Fillet the following edges with the parameters below:

   

   • Start a new sketch on the Front Plane, at the rear of the stock. Make sure to have Sketch1 visible.
   • Create the following sketch with the parameters below:

   

   • Cut-Extrude the profile with the following parameters:

   

   
   

   NOTE: At this point in the tutorial, you have enough details on your geometry to skip ahead to Step 4. To have a more complete looking stock at the end, please continue with this next list of features:

   
   

   
   

   
   

   • With the rear face of the stock selected, open the "Offset Surface" command and create it with the following parameters:

   

   • Start a new sketch on Plane 1.
   • Make sure to have the rear profile visible (it will be a sketch contained in our first loft feature).
   • Offset the profile 1.5mm to the interior:

   

   • Start the "Surface-Extrude" command and complete it with the following parameters:
   • NOTE: The two surfaces used to terminate the feature at both ends.

   

   • Select the highlighted face below and activate the "Offset Surface" tool. The input is 0.000 on purpose. Finish the command.

   

   • NOTE: I've hidden the main body of the stock for clarity in this next portion.
   • Select the "Trim Surface" tool and use the 'tubular' surface as the Trim tool to trim the outer edge of the front and back surface:

   

   • Knit the three remaining surfaces together:

   

   • NOTE: Make sure the main body of the stock is visible, if you hid it for clarity like I did.
   • Open the "Combine" tool and select the two solid bodies. Merge them with the following parameters:

   

   • Chamfer the edge with the parameters below:

   

   • Start a 3D sketch and convert the following profile to sketch entities:

   

   • Close the sketch and start a new one on the Top Plane.
   • Create the following sketch:

   

   • Finish the sketch and open the "Surface-Sweep" tool. Complete the feature with the following parameters:

   

   • Select the surface below, then open the "Offset Surface" tool, with a 0.000 input. Finish the feature.

   

   • Knit the two new surfaces together:

   

   • Open the "Cut with Surface" tool and cut the main body of the stock with the previous surface.
   • NOTE: The direction of the arrow is important as to which side to cut. If you cut the wrong direction, simply open the feature back up and flip the direction.
   • The finished feature should result in a chamfer.

   

   • Start a new sketch on the Top Plane with the following parameters:
   • NOTE: Make sure the previous contour sketch is visible for reference.

   

   • Finish the sketch and add the following reference plane:

   

   • Create the following sketch on the new reference plane:

   

   • Open the "Cut-Sweep" tool and finish the command with the following parameters:

   

   • Mirror the previous swept cut over the Front Plane:

   

   • Fillet the edges around both swept cuts with the following parameters:

   

   • After all of these features, your model should look like this:

   

   
   

   With our detailed part complete, we are now ready to turn it into a laminated stock!

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

4. Step 4: Laminating the Stock

   It's now time to create the laminated look we are going for. These next few steps are hardware-intensive to your system. Due to the power of my own system, I had to perform a feature in two instances instead of one. This may or may not work for you, depending on your hardware.

   NOTE: This only applies if you wish to save the slices as individual files. Saving the slices internally to the original file does not take up much system resources.

   
   

   
   

   • Start a sketch on the Top Plane and create this sketch:

   

   • Extrude the line as a surface with the following parameters:

   

   • Pattern the surface with the following parameters:

   

   
   

   NOTE: SAVE YOUR FILE AT THIS POINT!

   
   

   • Now open the "Split" tool and select all of the patterned surfaces, including the original.

   

   • Click the "Cut Bodies" button, and allow the list to populate. Then click the "Auto-assign Names" button.
   • NOTE: If you click the scissors icon in the "Resulting Bodies" field, you DO NOT have to click "Auto-assign Names". This will result in saving the slices internally to the current file.

   

   

   • Complete the command.
   • NOTE: SolidWorks will now generate every 'slice' of the model as an independent part file and open/save it. It is okay to close all of these open part files. We will deal with them later. *IF THE SPLIT FAILS*, close SW and re-open it. You will have to reduce the amount of cutting surfaces and increase the number of 'splits' you can do at once. This will all depend on your hardware's capabilities.
   • Your model should now look like this:

   

   • I have the original cutting surface shown above because we need to pattern it to the other side of the model now.
   • Pattern it over to produce another 'stack' of cutting surfaces:

   

   • Perform the "Split" command again using the previous steps.
   • NOTE: If the split fails, or SolidWorks Resource Monitor starts going off, close SW and reopen it. Reduce the number of cutting surfaces and try again.
   • With all of the generated part files closed, navigate to the folder where they were dumped. These are all individually editable if you require them to be.
   • It is SAFE to delete these files if you have no use for them. They do not effect your original file.

   

   • Assuming your split commands were successful, your model should now look like this:

   

   
   

   Congratulations! You've just created a laminated wood stock! To add some details to this part, proceed to the next step...

   
   

   
   

   
   

   
   

   
   

   
   

   
   

   
   

5. Step 5: Applying Appearances

   With the model complete, we can now have some fun with appearance. You can choose from anything you like in the SW appearance library, but I'm going to make mine out of some accurate-looking choices.

   
   

   
   

   • With the model being viewed from the top, right-click the 'middle slice' and select "Body" from the appearance drop-down.

   

   • This will open up the appearance property manager.
   • You can now proceed to select every other 'slice' and apply your desired appearance to those slices. I'm going with 'satin finished teak 2d':

   

   • Complete the command, then start the process over for the next set of slices. I chose 'satin finished mahogany 2d' for my second set.
   • If you chose the same appearances as I did, your model should look like this:

   

   
   

   Thank you for taking the time to view my tutorial. I hope it added a useful skill to your portfolio! If you have a request for another tutorial, leave a comment below and I'll see what I can do!