Drawings in AutoDesk Inventor 2014
mond.araba
instructions.zipH.W. 04/2D Drawing pdf may assist you.zip
2D Drawing pdf may assist you/A file may assest you to make the 2D drawing of HW 4.pdf
MEE 227L – Lesson 5 Orthographic Projections, Principle Views
Auxiliary Views, Detail Views, Section Views Thursday, February 6, 2014
Dan Price
University of Dayton
Orthographic Drawings
• Representations of 3-dimensional objects arranged in a standard manner so they can be easily understood by others familiar with the standard.
Orthographic Projection
• The primary views on a drawing are made using “Orthographic Projection”
• Orthographic Projection creates views of an object by projecting an “image” of each side or view” onto a plane that is parallel to that side by tracing a perpendicular line from each feature to the view plane
• Can also be imagined by drawing or tracing the shape/features of the face of the object onto an imaginary “glass plane” that becomes the view.
Orthographic Views
• Now unfold those views so they are all in the same plane as the “Front” view
• Now you have an Orthographic Drawing!!
Orthographic Drawing
• Start With a 3D Inventor Part • Create a Drawing With 3 Orthographic Views
Using Inventor to Make Orthographic Drawings
• With the Part Already Open • Select New On the Metric Tab, Pick ANSI (mm).idw
Start With A Completed 3D Part
• New drawing from template with borders and a title block. It will default to some size, such as C-size (17” x 22”)
• Change the size of the drawing sheet by right-clicking on “Sheet 1” and choosing “Edit Sheet”
• For example, change sheet size to A (8.5” x 11”)
A New Drawing With Borders
• The first view placed on a drawing is called the “Base View” • Click on “Base” to begin placing the first view
Now Place Views
• Pick the orientation of the initial view • You can open up a window to orient the base view in 3D • You may choose to adjust the scale of the view
• Most of your work should be 1:1, unless two big to fit on standard sheets, or so small that it doesn’t allow room for dimensioning, etc.
Base View Dialogue Box
• When you have what you consider to be the “Front” view, click to place the view on your drawing sheet
• The base view should usually be in the lower left corner
Place the Base View
• Many “prismatic” parts will require 3 views to define them • Select the “Projected” button to place orthographic project views • Then select the base view to project from • Move your cursor around the page to see which views you can place
Now Place Projected Views
• For each view, left-click to locate the view • Then right-click and select “Create”
Create Projected Views
View Display Options
• Right click on any drawing view and pick Edit View. . . • Pick the Display Options tab for options about what is
displayed or not
Special Case – Cylindrical Parts
• For a cylindrical part, a Front View and Side View would be identical
• Typically, only two views will be provided
Hidden Lines • To the extent “hidden” can be used to clarify the
drawing, they are shown as dashed lines • Do not use hidden lines that could tend to confuse
• For example, hidden lines for holes in a bolt circle are typically ONLY shown on the outside of the part where they help clarify the position.
Drawing Clean-Up
• To remove specific hidden (or even solid) lines, right click on the specific line and toggle off Visibility
• To restore all hidden lines, right click on the whole view and select “Show Hidden Edges”
Alternatively – Use Section Views
• These days, since it’s so easy to create sections, often a section view is used instead of hidden lines
• Where details are “hidden” by the outside shape of the part, Section Views can provide the necessary details about the part
• Begin by placing necessary base and projected views • Then select a view to section • The section will be perpendicular to the selected view and
section line
Section Views
• Now select the Section tool and click on the view from which the section will be “cut”
• Click to start and stop the line, aligning it with appropriate centerpoints • Be sure to extend line slightly outside the part • When complete, right-click and select “Continue” • Place the view in an initial location
Section Views
• Select your options in the “Section View” dialogue box • Make sure the light bulb icon is “lit”
• As you move your cursor, the Section View placement moves with it • Left click when you have the section view placed where you want it
Section Views
Auxiliary Views • When objects have surfaces sloping at angles to the principal
orthographic views, Auxiliary Views are used to show their features in “True View”
• Without Auxiliary Views, sloping-surface features won’t appear in their true size and shape, or “True View”
Auxiliary Views
THIS
NOT THIS
Auxiliary Views Are Still Projected Views
• In addition to the front and top views, we project a view onto a plane parallel to the sloping surface
• As with Orthographic Projections, we “unfold” the views • The Auxiliary view uses a “fold line” parallel to its edges
“Unfold” The Auxiliary Projection
• By convention, we don’t show the sloping view if it is better shown elsewhere in a True View Auxiliary View
• Inventor has tools for that (albeit flawed tools)
Auxiliary View Convention
• Start With a 3D Inventor Part That Has a Sloping Surface • Create a Drawing With relevant Orthographic Views
Using Inventor to Make Auxiliary View
• In the .idw drawing file, select “Auxiliary” from the “Place Views” menu
• Select an Orthographic View that shows sloping surface on edge
• Select that edge to define the Auxiliary View
Create Auxiliary View In most cases, select the view to NOT show hidden lines.
• Left-click to place the Auxiliary View • Use Inventor’s “Crop” tool to omit unneeded areas
Place the Auxiliary View
• On an Ortho view crop-out that which is better shown in the Auxiliary view
• Select the Crop tool and draw a rectangle around what you want to keep
• Repeat for the Aux. view, keeping just the True-View portion
Crop the Auxiliary View (As Needed)
• Sometimes a “closer look” is needed to provide details of an area
Detail Views
• After placing the first view, zoom in on an area where a Detail View is needed
• Click on the “Detail” tool under the “Place Views” tab
Detail Views
• Select the view • The Detail View dialogue
box opens • In the “View Identifier”
field, name the view • In the Scale field, select a
scale, such as 2:1 or 4:1 • Also select “Fence Shape”,
“Cutout Shape”, and “Style” • Normally we would not use
hidden lines in a detail view
Detail Views
• After clicking “OK” in the dialogue box, click to place the Detail View
Place the Detail View
2D Drawing pdf may assist you/MEE227L Lesson07 Assemblies.pdf
Lesson 7 – Assemblies Creating Assemblies from Existing Parts
Putting Assemblies in Motion
Tuesday February 11, 2014
Dan Price
Starting Point – Existing .ipt files After you have created component parts (.ipt files) that you want to include in an assembly, create a new folder that you will use for the assembly, and move the components to that folder. For this Lesson, you can find 4 component files on our Isidore site.
Starting Point – New Assembly (.iam)
1. Start a new document and select “Standard (mm).iam”, for example, to start a new assembly. Once you have started the new assembly, save it in the same folder where your component parts are.
Select The First Part 2. On the “Assemble” tab, click “Place” to select the first component that is
the most stable “base” of the assembly. When the dialogue box opens, navigate to your part, highlight it and click “Open”. This part will be “pinned” or non-movable.
Insert a Second Part
3. Now click “Place” again to put the second part into the assembly. 4. Navigate to the part you want to add and click “Open”
Place the Selected Part in the Assembly 5. Now a representation of the part will float with your cursor. Move the
cursor until the part is close to where it should be. Click to place the part.
6. If two or more repetitions of the part will be in the assembly, click multiple times to place more copies. Hit escape to finish.
Move and Rotate the Part to Near Where It Goes
7. On the Assemble tab, in the Position section of the ribbon, use “Move” and “Rotate” to position the second part close to where it goes.
Repeat Until All Parts Are In Assembly
8. Repeat until all parts of the assembly are on the screen.
Constrain the Parts To Each Other 9. Select “Constrain” to open the “Place Constraint” diaologue box. 10. In most cases, we will use the first button (“Mate”)
Select Mating Features to Constrain 11. Now select the feature on the part we are moving. In this case, we want to
align the inside wall of the slider with the side wall of the caliper. Select the 12. You might have to use the selection tool to get to the exact feature you need.
Always click “Apply” or “OK” after you have the constraints you want.
Select Additional Mating Features 13. Now select other mating feature on the base part and mating part until
you have the degree of constraint appropriate for the assembly. Here I am mating the flat surface of the slider to the “back” face of the caliper.
Constraining Axial Features 14. Some parts you will want to line up axis-to-axis, like this knob and the
hole in the slider. In this case, be sure to select the CENTERLINES, not just the centerpoint of the circular edge!
Flush Mating Condition 15. Some parts instead of mating face-to-face, you will want them lined up
flush to each other. Click the “Flush” option button in the “Place Constraint” panel, then select the two faces you want lined up.
16. Continue to add constraints until you have all parts lined up as you want.
Look at the Effects of the Constraint
17. AFTER applying the constraint, hit “Esc” to get out of Constraint mode. 18. Now take your cursor, hover over the Slider part, then left-click/hold.
Now move your cursor around to see how your part can still move. 19. In this case, the slider will slide along the rectangular shaft of the caliper,
but it always stays aligned. Also, the knob is free to spin about its axis
Add a Constraint to Prevent a “Crash” 20. Right now, the Slider can “crash” into the blade of the Caliper 21. Add a mating condition to prevent the crash while still allowing motion
Add a Constraint to Prevent a “Crash” 22. Select the two small faces of the opposing blades 23. Click the >> button to expand the Place Constraint panel 24. Check the box for “Minimum” under Limits, then click apply. Now you can still
move the Slider, but it won’t crash into the Caliper 25. See what happens if you click the “Use Offset As Resting Position” option
Note: View is changed to Perspective mode in this shot
A Few Words About Assembly Files • For this assembly and its components, notice the file size of the Assembly
(.iam) • The assembly file is smaller than both component files • The assembly file DOES NOT contain the part geometry • ALWAYS KEEP THE ASSEMBLY FILE TOGETHER WITH ITS PARTS • They must stay in the same relative folder structure • When you hand in an assembly YOU MUST keep all parts together in the
original relative folder positions • One easy way:
• Start with your component parts in the same folder • Save your assembly in the same folder as the components • To hand the project in, zip the folder and upload it (7-Zip is a great tool)
Fun With Assemblies - Motion • It’s fun to simulate motion in an assembly • It’s easy to simulate motion in an assembly • You use constraints with an offset, and then drive the constraint through
a range of offsets to simulate motion
Start With A Complete Assembly • Start with a completed assembly that “wants” to have motion, such as
our Slider moving along the shaft of the Caliper • We can “slide” the Slider along the Caliper • In this case, we already put on a mating constraint that we can use for
this: the constraint between the small faces of the opposing blades (Step 22 above). Right click on that constraint in the model browser and select “Drive”.
Drive the Constraint to Move the Parts
• Now enter in the distance between the two mating surfaces in the closest and farthest positions, in this case 0 mm to 50 mm. Click the play forward (>) and play rewind (<) buttons a few times to see how it works.
• Now click on the >> to show the bottom panel
Now Record the Motion Simulation • Make sure “Minimize dialog during recording” is checked • The animation MAY be smoother if the AVI rate is a whole-number factor of the total number of steps • Click on the red Record button to open the record file and properties panel • Save as an .wmv file, not .avi, or just play with it to see what works best • Click the run arrow to begin the animation and the recording • For linear motion that stops and starts at the same point, click Start/End/Start, and enter 2 in the field. • Click Play (>) to initiate the recording. The images take a while to render, so please BE PATIENT!
Simulating Rotational Motion These instructions were for different parts, but they apply to our parts. See if you can make them work for our assembly • Let’s create a constraint between one of the knurl faces of the knob and one of the
narrow vertical faces of the piston • Notice the options I chose in the Place Constraint panel • After you click “OK”, notice that you can no longer “spin” the wheel manually
Now Drive That Constraint • Find that new constraint in the assembly browser • Right-Click, then select “Drive Constraint” • Click the >> to expand the Drive Constraint panel fully • To spin the knob 10 rotations, enter “3600 deg” in the End field • Type the number of steps from min to max, and 2 under Start/End/Start • Under “total # of steps” enter some whole factor of the “End” value
Now Run the Motion Simulation
• Click the Play (>) button and watch the motion simulation. • Tweak any parameter as needed (Play!)
Now Record the Motion Simulation • Find the .wmv file you created • Launch the file in your favorite media viewer • You can also paste it into PowerPoint and other applications (sometimes it works)
2D Drawing pdf may assist you/MEE227L Lesson08 Assembly Drawings.pdf
Lesson 8 – Assembly Drawings
Tuesday, February 18, 2014
Dan Price
University of Dayton
Assembly Drawings • Creation of assembly drawings is not much different than creating
drawings of individual parts. • For example, we can easily place 3 views of our Caliper Assembly.
Assembly Drawings • You can place base and project views, section views, auxiliary views,
detail views, etc. • You can also place special views very helpful for specifying assemblies.
Assembly-Specific Views Break-Out View: For example, you can create a Break-Out view where you show a dimension between two parts not otherwise visible.
Break-Out Views
1. In this case, I started with a version of our Caliper assembly saved with the jaw opening at 10 mm. (How did I do that?)
Break-Out Views 2. I placed a new BASE view on my sheet, referring to the caliper
assembly with the 10 mm jaw gap. (Note: Not all views on a drawing have to be from the same part!)
3. I oriented the view using the Change View Orientation tool
Break-Out Views 4. I rotated the assembly to the view I needed, then clicked “Finish
Custom View.” 5. Back in the drawing, I placed the view on the drawing.
Break-Out Views 6. With the new view selected,
click the “Create Sketch” tool 7. Use the Spline tool to create a
closed shape around the area you want to cut away.
8. Click Finish Sketch
Break-Out Views 9. Now select the Break Out tool 10. Select the view in which you just placed the sketch 11. Click the Profile selector and select your new sketch There are various ways to select the Depth. What’s right for your view depends on the parts. Basically pick a point on the same depth level as you want to show.
Break-Out Views
12. In this case, I select the “From Point” method and chose the edge indicated below
13. I chose 0.000 depth from that point to get a view of the parts that are right at the same depth as the edge of the shaft of the caliper.
Break-Out Views
14. This results in the “hybrid” view shown: Part break-out, part section
15. You can tweak your break-out fence by editing the sketch
Assembly Drawing Parts List Inventor has a nifty tool to create a Parts List for an Assembly Drawing 1. In the drawing file for the Assembly, on the Annotate ribbon, click “Parts
List”
Assembly Drawing Parts List, Cont’d
2. In the Parts List panel, click the Select View button, then click on a view that shows all or most of your component and/or subassembly parts. A section view, breakout view, or an exploded view (we’ll cover this later) is usually a good choice.
Assembly Drawing Parts List, Cont’d 3. In the Parts List panel, under BOM View, select Structured and under
Levels, select “All Levels 4. Click the “Select View” tool, then select the view you want to base the
Parts List on 5. Click “OK” 6. If you get a warning as show, click OK again.
Assembly Drawing Parts List, Cont’d
7. After you click “OK”, you need to show Inventor where you want to place the Parts List.
8. You will be shown an outline of the size of the Parts List. I normally place the parts list along a border.
Assembly Drawing Parts List, Cont’d
9. To format the Parts List, such as adding, deleting, or widening columns, right-click on the parts list and select “Edit Parts List Style”
10. You can choose which columns show up , how wide they are, the heading of the parts list, etc.
Expand the Parts List 10. Double-click the Parts List itself to edit it (or right-click and “Edit Parts List”)
11. Click on the + signs to expand out all levels as needed 12. Part Number and Description come from iProperties for each part. If
you didn’t fill that out, best do it now in the part. You can edit it here, but it doesn’t “stick” with the parts
Now the fun part. . . Now that you have a Parts List, you can add Item Balloons to identify the parts on the Parts list. 1. Still in the Annotate ribbon, on the Balloon tool, select Auto Balloon 2. Click “Select View Set”, then select the view where most/all your parts
show up
Item Balloons, cont’d
3. Now click “Add or Remove Components” 4. In the view, use your cursor to place a rectangle around all parts to
select them, or select/de-select them one-by-one
Item Balloons, cont’d 5. Now click “Select Placement” 6. Select “Around” as the placement type 7. Now as you move your cursor around, the position of the balloons will
adjust. Find the location that pleases you the most. 8. Click OK to set the balloons
Item Balloons, cont’d 9. Each balloon corresponds to one of the items in your parts list. 10. Item numbers are used instead of Part Numbers because part numbers
can change. 11. You can adjust the balloon positions one at a time
2D Drawing pdf may assist you/MEE227L Lesson09 Assembly Exploded Views.pdf
Lesson 9 – Assembly Exploded Views
Thursday, February 20, 2014
Dan Price
University of Dayton
Assembly Exploded Views You can show a lot about how an assembly is put together using section views, parts lists, and item balloons. But it is hard to beat an exploded view to show how an assembly is put together.
Let’s Get Started A New File Type: To create an Exploded View of an assembly, Inventor requires that you create a new file in a new file type called a Presentation. Select New File, then navigate to the Standard (mm).ipn template.
Select The Assembly File 1. Select Create View 2. In the Select Assembly panel, navigate to the Assembly you want to
explode 3. Choose Manual or Automatic. We’ll do Manual in this example, but also
play with Automatic.
Orient the Assembly
4. Orient your assembly so that the exploded parts will have room to explode. You can rotate, zoom, etc., as you go.
Tweak the Position of Your Parts
5. Under the Presentation tab, click “Tweak Components”.
6. Click on the “Direction” arrow, then select a feature or face on which to anchor an XYZ coordinate system.
7. Now click on X button 8. Click on the
“Components” arrow, select the Knob, Slider, and Pin, then slide them off the Caliper along X
Work Through All The Parts
9. One-by-one, select a component or components to move together or separately
10. Use the Direction button to move the XYZ coordinate system that can help you orient the direction of the explosion
Position Parts in Groups or Individually
11. See the difference between selecting one vs. multiple components together
12. Select one component to move it independently; select several to move them together
Offset Components 13. By choosing a different axis and moving the part along that axis, you can offset
one or more of the components to make the explosion easier to see. 14. You can further tweak the offset components by selecting the Edit Existing Trail
arrow, then select and adjust the Trail handles.
You Can Animate It
15. Inventor allows you to animate the explosion, but it remembers EVERY move you make
16. This is probably a better option if you have used the Automatic Explosion, but for many assemblies the Automatic Explosion doesn’t work well
Auto Explode
17. Sometimes Auto- Explode is HORRIBLE ! !
18. This is what I got when I auto-exploded our Caliper Asm
19. But you can also start with an Auto-Explode, then tweak
Show Your Exploded Assembly In A Drawing
20. Save your exploded view file (.ipn) 21. Now add a view of your Exploded Assembly in a new drawing or
on a new view or sheet in an existing drawing 22. For a new drawing, select New File, then use the ANSI (mm).idw
template
Add a View of Your Exploded Assembly 23. Add a Base View and navigate to the .ipn file your exploded and saved 24. Use the Change View Orientation Button to position the view 25. If you created more than one explosion in your .ipn file, select the one
you want.
Add a View of Your Exploded Assembly
26. Place and adjust the position of your Exploded View 27. From there, you can create a parts list, use balloon parts labels,
and add any other notes or even assembly instructions.
2D Drawing pdf may assist you/Piston Gripper Asm.pdf
SECTION A-A
SCALE 1 : 1
A A
PARTS LIST
DESCRIPTIONPART NUMBERQTYITEM
PISTON ASM000111
CYLINDER BODY000511.1
BASE - PISTON000211.2
CAP - PISTON000311.3
PISTON000411.4
SIDE PLATE000511.5
LINKAGE ASM - PISTON001012
LINK - PISTON001912.1
SHORT LINK ASM002022.2
LINK - SHORT STRAIGHT001112.2.1
BUSHING - STEP, .157 X .375001242.2.2
GRIPPER LINKAGE ASM001323
LINK - GRIPPER002113.1
ANGLE LINK ASM - BUSHING001413.2
ANGLE LINK001513.2.1
BUSHING - STEP, .157 X .375001243.2.2
LINK BUSHING ASM - LONG001613.3
LINK - LONG STRAIGHT001713.3.1
BUSHING - STEP, .157 X .375001243.3.2
1
1
2
2
3
3
4
4
A A
B B
C C
D D
SHEET 1 OF 1
DRAWN
CHECKED
QA
MFG
APPROVED
OBERMEYER J
11/6/2011
DWG NO
Piston-Gripper-Asm
TITLE
PISTON GRIPPER ASM
SIZE
C
SCALE
UNIVERSITY OF DAYTON
REV
001
REVISION HISTORY
ZONE REV DESCRIPTION DATE APPROVED
N/A
001 INITIAL RELEASE
11/6/2011
CN001
3.1
3.2.2
3.2.1
3.3.1
3.3.2
2.2.1
2.2.2
1.5
2.1
1.3
1.1
1.4
1.2
2D Drawing pdf may assist you/Rules of Dimentioning on the 2D drawing.pdf
MEE 227L – Lesson 6 Dimensioning Review
Thursday, February 6, 2014
Dan Price
University of Dayton
Dimensioning • Drawings use dimensions and notes to show the size and
specifications of a part and any other information needed to manufacture the part.
Dimensioning Terminology
Dimension Line
Leader
Extension Line
Section Line
Centerline
Dimension
Tolerance
GD&T
Dimension Orientation
• 2 Styles: Aligned or Unidirectional
Aligned Unidirectional
1. First row of dimensioning is 3 X Letter Height from the part (minimum), and 2 X Letter Height apart
19 Rules of Dimensioning
2. Place Dimensions between the views
19 Rules of Dimensioning
3. Dimension the most descriptive views
19 Rules of Dimensioning
4. Dimension from visible lines, not hidden lines.
19 Rules of Dimensioning
5. Give an overall dimension and omit one of the chain dimensions.
19 Rules of Dimensioning
6. Organize and align dimensions for ease of reading.
19 Rules of Dimensioning
7. Do not repeat dimensions.
19 Rules of Dimensioning
8. Dimension lines should not cross other lines.
19 Rules of Dimensioning
9. Extension lines may cross other lines if they must.
19 Rules of Dimensioning
OK
10. Do not place dimensions within the boundary of the part unless absolutely necessary.
19 Rules of Dimensioning
OK
11. Place angular dimensions outside the angle with extension lines.
19 Rules of Dimensioning
12. Dimension rounded corners to theoretical intersection.
19 Rules of Dimensioning
13. Dimension cylinders with diameters: a. Dimension holes in circular view b. Dimension cylinders in rectangular views
19 Rules of Dimensioning
14. Stagger numbers to prevent crowding.
19 Rules of Dimensioning
15. Hole sizes are best given as diameters with leaders in circular view.
19 Rules of Dimensioning
16. Leaders should have horizontal elbows and point toward the hole centers.
19 Rules of Dimensioning
Horizontal Elbow
Leader would cross through center
17. Extend leader from the first or last word of a note.
19 Rules of Dimensioning
CHAMFER 4 X 4
BOTH ENDS
CHAMFER 4 X 4
BOTH ENDS
CHAMFER 4 X 4
BOTH ENDS
CHAMFER 4 X 4
BOTH ENDS
19 Rules of Dimensioning
18. Dimension arcs (less than 180°) with Radii (not Diameters)
19 Rules of Dimensioning
19. Locate holes in circular views (to hole center NOT edge!) and dimension diameters with a leader
Dimensioning Circles and Arcs
• To dimension circular and arc-shaped items in Inventor, you first will usually add centerlines
Dimensioning Circles and Arcs • The tool in Inventor for placing centerlines is under the “Annotate” tab. • The cross-hair centermark is for holes, cylinders, and arcs in their true-view
(true circles and arcs) • Click on the centermark tool, then click on the arcs and circles
Dimensioning Circles and Arcs
• Next click on the centerline tools to mark centerlines that connect arcs and circles, and centerlines of holes and cylinders in side view.
Dimensioning Circles and Arcs
• Next click on the centerline tool to mark centerlines that connect arcs and circles, and centerlines of holes and cylinders in side view.
Dimensioning Circles and Arcs
• Now you can use those centermarks and centerlines to place dimensions on your views.
Dimensioning Circles and Arcs • Equally-spaced holes on a common diameter (bolt circle) can be
dimensioned by giving the diameter of the bolt circle and the size and number of holes in a note with a leader to one of the holes.
Dimensioning Rounded Slots
• Dimension rounded slots with the overall width of the slot and the length only between the centerlines.
Editing Text • To add notes, such as “TWO PLACES”, right-click on the dimension after it is
placed. Edit text in text edit area. Use buttons in dialogue box to add symbols, etc.
• “Play” with this until you are comfortable using the tool.
Changing Dimensioning Style • To edit the format of ALL your dimensions, right-click on a dimension and select
“Edit Dimension Style” • On the Units tab, change the Precision from 2.12 to 1.1 • Click Save at the Top and Done at the bottom to save the change
Other Tips and Guidance
Counter-bore Holes: Give small diameter and depth, then counter-bore note or symbol and large diameter and depth.
Other Tips and Guidance
Counter-sunk Holes: Give small diameter and depth, then counter-sink note or symbol and outside diameter and included angle.
Other Tips and Guidance • Use Inventor’s Hole tool to create holes in your 3D design
• Use the Hole and Thread tool to dimension your Drawings
• Inventor will take care of the details
1. Right-click in the view where you are having problems, then select "Retrieve Dimensions“
2. Next, click the Select Dimensions button, then look for the dimension you need. When you click on it, it will stay with your view. If you don't find the dimension you are looking for, there is some chance that your 3D model is actually wrong.
3. You can use this feature for ALL dimensions.
Other Tips - Retrieve Dimensions
Other Tips and Guidance
• Material Notes: Material designation and type of finish (coating or plating) is given as a note either within the title block or near the title block.
• Tolerance Block: Default tolerances should be specified in a general note either within the title block or near the title block
Other Tips and Guidance
• The size of multiple features in the same view can be specified with a single dimension and note
Editing Title Block Fields, cont’ • The content of the fields for the Title Block are controlled by “iProperties” • Click Start iProperties • The “Summary” tab contains the drawing “Title” and “Author” (DRAWN), and
“Company” fields
Editing Title Block Fields, cont’ • The “Project” tab contains the drawing “Part Number” (DWG No.), “Revision
Number” (REV), and “Creation Date” fields. • The creation date defaults to the data the file was last edited, but can be
manually changed.
