AutoDesk Inventor: Creating Working Drawings Inventor allows you to quickly and easily make quality working drawings from your 3D models. This tutorial will walk you through the steps in creating a working drawing. You will notice throughout this tutorial that ANSI is mentioned quite a bit. ANSI is the acronym for the American National Standards Institute and, in drafting, they have created a set of rules of how drawings should be made including line weights, text sizes, dimension styles, etc. 1. Open a New Metric Drawing File. Use the ANSI (mm).idw You will be using metric, but make sure when you start a drawing that it is in the same units as your model. Save As. YOURNAME_CRADLE SUPPORT.idw 2. You will notice a few changes on the screen a. The Model Space is now Paper Space complete with a title block and border. b. The Browser has a few new headings. c. The Ribbon has some different features.
Setting up the page 3. You may notice that the sheet looks rather large. In the Browser, right click on Sheet 1, and select Edit Sheet. This opens a dialogue box where you can change the settings for the sheet you are creating. 4. Change Sheet Size to A. Notice how the Height and Width change to 8.5 and 11, which the size of a standard sheet of paper. Click OK. 5. The Title Block now looks a lot larger in comparison to the paper. In the Browser again, right click on the ANSI Large heading and select Delete. 6. Under Drawing Resources in the Browser, click the little plus sign beside the heading Title Blocks. A few standard options show up, right click on ANSI A and select INSERT. You now have a standard A sheet title block. 7. Delete the Default Border under Sheet 1, right click and Insert a new Default border. 8. A dialogue box will appear, select None for both the Vertical and Horizontal Zones. This removes the numbers and letters from around the border. 9. Next go into the main Inventor menu and select iproperties. This brings up a dialogue box that allows you to add characteristics of the project.
10. Under the Summary tab, add your name where it says Author. Add CRADLE SUPPORT where is says Title, and add SARDIS MECHANICAL where it says Company. Click OK. This automatically adds these to the fields in the title block of your drawing! 11. Your sheet is now ready for the drawing. Inserting Object Views 12. In the Ribbon, under the Place Views tab, click the Base option. 13. This opens the Drawing View dialogue box. This box gives you options and tools to insert different views of a chosen model. 14. Use the file browser and open your Cradle Support model. That was the model you created right after the first tutorial 15. Set the Scale at 1:1. This is the size of the drawing in relationship with real size of the model.
16. Move the Drawing View dialogue box to the left and Pan the Sheet so that you can see the left half of it. This will help when placing the views. 17. Select the Front view from the Orientation list. Move your cursor over the Sheet and you will see the shape of the object from an orthographic view. 18. Click to place this view in the lower left corner of the Sheet. 19. The dialogue box will disappear and the Front view will be seen as a line drawing. 20. Next the program wants you to place other views that are needed in the drawing. 21. Move the cursor directly above the front view and click to place the top view. Move the cursor to the right of the front view to place the right side view. 22. Right click anywhere and select Create to finish making the views.
23. You now have the three basic views of an orthographic drawing. 24. You can move around the views to arrange them nicely on the sheet. Do this by hovering over the view, a red border will appear, then click and hold the border to move. Since these are orthographic views, the other views will automatically line up with the one that is moved. 25. Insert a Projected isometric view in the top left corner so that the plan is easier to understand. 26. Click the Projected option from the Ribbon. 27. Select the Front view and move the cursor to the top right of the page. This will automatically insert an isometric view. 28. Click where you want it, then right click and select Create. The view is far too large to fit on the paper. 29. Right click on the isometric view s border and select Edit View. 30. This will bring you back into the Drawing View dialogue box. 31. In Scale, change the scale to 1/2. 32. The isometric view will shrink to half size, then you can place it in the corner for reference.
Creating a New Title Block 33. It appears that our sheet is quite packed with objects. This Title Block really is too big for what we need and has too many unneeded fields. Create a new title block that copies this one. 34. Right click on ANSI A title block in the Browser and delete it. 35. Right click on the Title Blocks heading under Drawing Resources in the Browser and select Define New Title Block. 36. This will open up some Sketch tools in the Ribbon. Draw out the shape above. Don t worry about its location, you can draw it anywhere. The narrow inside lines, and the diagonal lines on the company and title spots are for construction only. Click the Sketch Only option when drawing those lines. This will allow them to not show in the finished product. 37. For the Text, you will be adding regular text, and text with Properties. In the above drawing, the text that has the angle brackets (<AUTHOR>) around it is text with Properties. This allows the program to automatically add text into that location. This is where the words that you entered in iproperties end up being placed. 38. To create the Text with Properties, click the Text tool and choose the start point for the text (it can be moved after). 39. A dialogue box will open, instead of typing in words, choose Properties Drawing from the Type menu and then choose the required option from the Property menu. Click the Add Text Parameter button and click OK.
40. Use a height of 2mm for the regular text and 3.05mm for the text with properties. 41. Try to align the text so that it is well lined up. Center the Company and Title text in the opening. 42. You can change where you can locate the text from by playing with the options in the top left corner of the dialogue box. 43. Once everything is where you want it, click Finish Sketch. A box will show up where you can enter the name of your title block. Click Save. 44. You can now select your new title block from the Drawing Resources and insert it into the drawing. 45. The iproperties should have automatically filled in the required fields based on the information you added in the first title block. You will need to add the Scale manually. 46. There is now a lot more room to create all of your dimensions. Dimensioning the Drawing There are a few different ways to add dimensions to a drawing. 47. Right click on one of the views that you want to add dimensions to. In the list, select Retrieve Dimensions.
48. Dialogue box will appear. The view will already be selected as the view that you chose. 49. Click on Select Dimensions. A bunch of dimensions will appear automatically on the drawing view. Using the cursor, select the dimensions that you want to keep in the view. They can be moved around better after. 50. Click OK when done. 51. This is one way to add dimensions. Often though the program doesn t add them in the perfect spot that you want them. This is a good way to apply all the necessary dimensions, then come back and adjust and change their location. 52. In the Ribbon choose the Tab that says Annotate. 53. This will give you a bunch of tools for creating dimensions and text. 54. The Dimension tool will allow you to add a single dimension. It works with linear, angular, radius and diameter type dimensions. Click the button and then choose the parts places to measure. 55. Use the Baseline dimension tool to create a series of dimensions all on the same side at one time. 56. Click the Baseline tool, then click on the outer line of the part you want to dimension. Then click all of the points or lines that you want to measure to along the way.
57. Once all the lines are selected, right click and select Continue. 58. All of the chosen dimensions will automatically appear and arrange themselves. Move your cursor until the dimensions are in the correct distance from the view. The program has built in stops to automatically locate the distance that the dimensions are away from the view and from each other. When the lines snap into place and go dotted, then they are in the correct position. 59. There are several more dimension tools that make certain types of dimensions easier and faster to place. Play around with them. 60. Inventor has a built in command for dimensioning holes and other features that have been added to a model. 61. Click the Hole and Thread option and then click on a hole that has been placed in the model. This does not work on extruded holes, only ones that have been made with the Hole feature. 62. Click on the hole that you want to dimension. Drag the cursor and click to place the location for the text. Notice that it automatically added how deep the hole is. *THRU* 63. Use the Center mark and Centerline tools to automatically add these parts to the drawing.
64. Using all of these commands, add all of the necessary dimensions to your drawing. Look in the Mechanical Drafting pages 107-136, for all of the standards for mechanical drawings. All dimensions should be on the inside of the parts, not between the part and the border, if it can be helped. All arcs and holes should have center marks and centerlines, and be dimensioned to these. Make sure the location and size of everything is included. Don t repeat any dimensions. Once completed, create a working drawing for each of the first four tutorials that you completed. Each one may require different views to be able to fully describe the part.