Sheetmetal Parts at Harris: Preparing Files for Fabrication

This page documents how to prepare CAD-generated files for Sheet Metal Parts to have them fabricated at the Harris shop. Please carefully read the Fabrication page for the overall process of submitting parts to Harris! The steps here are a small subset of those overall instructions.

Check part's compliance with Harris rules

Verify first that the part has been set up to match Harris metal thickness and bend radius settings. You should've done this shortly after creating the part! See the requirements and instructions at Sheetmetal Parts at Harris.

Preparing files for Submission

We need two types of drawings for Harris:

1. pdf
2. dxf

pdf files – Step by Step Creation

1. STOP: Be sure a mentor has approved your part to make a drawing before proceeding. Check the parts log on google docs.
2. Open Inventor – you will be using this as a tool to make the .pdf file. We do not need to send the Inventor .ipw file to Harris.
3. Browse to the "[year] Build Season (ROBOT)/10 Shop Drawings" folder on the Robotics classroom share. Open the “[year] Drawing template”
4. IMMEDIATELY do a SAVE AS, specifying an appropriate name for your part's drawing.
5. Make the following edits to the basic drawing information:
   1. Fill in the Title Block - Expand "Sheet 1" in the document tree, expand "ied", double click "Field Text":
      1. Title: Should match exactly the Part and Assembly File Log title beginning with the part number.
      2. Date: This must be updated each time the part is sent – it tracks revisions.
      3. Your name here: Name of student who is making the drawing
      4. Mentors Name: Name of mentor who has reviewed the drawing.
   2. Edit the 'Notes section of the drawing - it is on the lower-right of the drawing. Double click it to edit as follows:
      1. Quantity Required per Robot: Fill in the total quantity needed PER ROBOT
      2. Material: Leave this as 0601 Aluminum. If you think you need something else, consult a mentor.
      3. Thickness: Aluminum sheet thickness. Use one of the Harris standard sizes: .032, .040, .062, .093, or .125 (DO NOT JUST RANDOMLY CHOOSE ONE OF THESES; the thickness should match your part's sheet metal settings, see Harris Sheetmetal Design considerations
      4. Bend Radius: Leave this as .032! If you think you need something else, consult a mentor.
      5. Finish: For unpainted parts, leave as "None". If the part is to be painted later by us, you can fill in paint color here.
   3. Open the model part file if it is not open (it must be open to place it).
   4. Check that the model file has sheet metal defaults as follows:
      1. Unfold rule is “Harris Shop”
      2. Thickness is a Harris standard (see Harris Sheetmetal Design considerations).
   5. Now place views to best represent the part on the drawing:
      1. Start by clicking Base and placing a TOP view (should be the flat top-down view)
      2. Click Projected and create side views off the top view as needed to show critical dimensions
      3. Consider also placing an ISOMETRIC view if it seems that would be helpful.
   6. Dimension Overall length, width and height of the part
   7. Dimension all hole diameters:
      1. Precision to three places
      2. For holes of the same size in the same area, use the “x 4” type of notation to indicate multiple hole locations
   8. Dimension each bend – height and angles other that 90 degrees. Dimension from outside to outside for bends!
   9. Indicate any PEMs or Rivets that Harris will be installing with the appropriate part number or size call-outs. YOU DO NOT NEED TO DO ANYTHING HERE IF ALL YOU WANT IS RIVET HOLES FOR RIVETS WE WILL INSTALL LATER.
   10. Save the drawing (.idw) to the 10 Shop Drawings folder
6. Save the drawing as a .pdf file:
   1. EXPORT as a PDF
   2. Save it to the 10 Shop Drawings/HARRIS PDF DXF FILES folder
   3. When sent to Harris, they will be moved into a “sent [date]” folder.
7. Print 2 copies of the PDF and put in the both together into proper section in the shop drawing red binder in the shop closet.

.dxf Files – Step by Step Creation

1. Start a new standard .idw drawing file in Inventor - use the Standard.idw template. Do not use the 1511 Sheet Template for generating .dxf files!
2. Delete the border, title block, and any other lines on the sheet before proceeding.:
   1. Expand "Sheet 1" in the document tree.
   2. Select "Default border" and press delete on the keyboard
   3. Select "ANSI Large" and press delete on the keyboard
   4. When you are done you should have a completely blank sheet!
3. Click BASE in the tool bar. Verify your part is in the "File" box or select it if not (you must have your part open in Inventor for it to show up)
   • Select Flat Pattern under Sheet Metal View. If the flat pattern is not available, go back to the model file and create a flat (unbent) version of the part.
   • Set the scale to 1:1
   • Adjust sheet size as needed so that the entire part will fit on the sheet. Reposition it by dragging as needed.
   • Click 'OK'
4. You should now have just the top view of the flat pattern on an otherwise blank sheet. The entire part should fit on the sheet!
5. If your part has bends, you will see the bend lines represented as dashed/dotted lines. These need to be removed before proceeding!
   • Click a dashed bend line in the drawing. Right-click and select "Visibility". The line should disappear.
   • Repeat for all bend lines on the part.
   • Alternatively, you can also hold CTRL and select multiple lines and toggle the visibility all at once.
6. Save the drawing:
   1. Go to SAVE A COPY AS and change the “file types” to .dxf
   2. Click the “OPTIONS” button to the left of SAVE
   3. The OPTIONS menu will appear.  Click on the drop down menu called “File Versions” and select “AutoCAD 2000/LT2000 DXF”.
   4. Without changing any other settings, click “Next” and then click Finish”
   5. Save it in the 10 Shop Drawings/HARRIS PDF DXF folder.
7. Update Part & Assembly File Log on Google Drive