SOLIDWORKS TO LASER CUTTER DOCUMENT CONVERSION

Transcription

1 UNIVERSITY OF CALIFORNIA, SANTA CRUZ BOARD OF STUDIES IN COMPUTER ENGINEERING CMPE118(218)/L: INTRODUCTION TO MECHATRONICS SOLIDWORKS TO LASER CUTTER DOCUMENT CONVERSION PURPOSE: This document outlines the procedures to convert your SolidWorks assembly file into a document that can be sent to the laser cutter. This procedure has substantially changed from our previous methods. The result of following the instructions in this document will produce a file ready to be cut on the laser cutter, which will dynamically accept changes to material thickness, and be very easy to modify going forwards. OVERVIEW: As part of the CMPE118 class, you will be modeling your robot in SolidWorks, and cutting your parts out of foamcore, MDF, or acrylic. SolidWorks is a very capable 3D modeling program which allows you to design and assemble your robot on the computer, make sure everything fits together, and inspect everything before you have a physical part. To get to the physical parts, we use a laser cutter to cut the 2D shapes out of our approved materials. This document assumes you already know how to use SolidWorks, and need only be guided on the specific steps needed to create a cutting document. You will be creating a new assembly with all of the parts you need to cut out for your robot on a single flat plane with distances between them. By using the mates in SolidWorks to generate this, the parts will dynamically scale with changes in material thicknesses. It will also remove the error of having differing parts at differing scales (which is a common way to mess up). You will be exporting the file as a DXF file, which is then used by the laser cutter software, RDWorks. All of this should substantially improve the laser cutting process and make it go much faster. PROCEDURE: In this section, we will go through the specific steps needed to create the cutout assembly in SolidWorks, and export the file to DXF format for the laser cutter (and how to ensure that it is a valid file). We will be using a rather simple foamcore tray as our example which has three distinct parts, but requires 2 copies of some of the parts for a full assembly. You are free to lay your parts out in any fashion that makes sense to you, and does not waste material. Also note that the distance mate that will be used can accept a variable in case you want to define it in a single place. Instructions on how to manipulate SolidWorks are available on the class website. They also have excellent tutorials online.

2 1. Open your final assembly in SolidWorks: 2. Create a new assembly. File->New->Assembly. You will want to save the new assembly file with a descriptive name. 3. Insert the first part into the new assembly. For this you will use the Insert Components tool, and browse for the part name. Once you have selected your part, it will float inside the main window. Click on the green checkmark in the insert pane, and the part will be placed on its drawing defined plane (see image). 4. This first part will now be inserted into the new assembly. You should not need to manipulate it further. It is listed in the Assembly menu on the left.

3 5. You can use the parts explorer (small folder on the right) to view all of the parts in the assembly. You can drag and drop parts from this to the cutting assembly. Do this with as many copies of the parts as you need in your robot. 6. At this point, you should have an assembly with all of the parts you need to cut out. You will use mates to create the layout with all of the parts you need to cut out for your robot laid flat, and without any overlap. You are free to lay out your parts in any way that makes sense to you and

4 conserves the material you are cutting. Doing it this way ensures that everything is at the same scale and that your parts don t overlap. 7. Mate the parts together so that they all have the same plane, and that they don t overlap. Mate the surfaces coincidently, and any convenient edges to place the parts the way you want to cut them out. This is something you should already know how to do. You will need to do this for all of the parts that you want to cut out until the entire set of parts is mated to your initial main part. 8. You will need a distance mate between the inner face of one part and the outer face of the other. This is what will keep the parts from overlapping when you change material thickness or other variables within your main assembly. Note that the distance can be set as a number, or defined as a variable. You might need to play with the mate alignment and flip dimension checkbox to have it go the right way.

5 9. Repeat this process for all parts until the entire set is mated to each other in such a way as they will not move when you try to drag them. You cutting assembly is now well defined.

6 10. Save your assembly file. This will be the file from which you generate the drawing that is actually used by the laser cutter software. Note that if you modify parts in your main assembly, these will automatically update in the cutting assembly as well. If you create new parts, they will need to be added to your cutter assembly. 11. With the flat assembly open, File->make drawing from assembly. The assembly of flat parts will be there in the pane on the left. Generally the one you want is the top view. You will want to turn off layouts, and drag it onto the page.

7 12. Make sure that you set the scale to custom, 1: Save the file as a drawing file, and save as a >DXF file for exporting to the laser cutter. To verify that the DXF file is correct, open it with edrawings application (the lines will show white on black). You should see the layout that the laser cutter will cut.