Jump to content
JD Mather

Inventor 101

Recommended Posts

JD Mather

Horizontal Midpoint.PNG

 

Add a Horizontal constraint to the angled line and then change to Construction linetype.

 

Drag a corner of the rectangle - notice that is stays symmetrical top-to-bottom about the origin. Creating symmetrical relations like this is the key to Inventor sketching.

 

Exit sketch and save the file as Punch Base.

Share this post


Link to post
Share on other sites
JD Mather

Dimensioning.PNG

 

Dimension as shown.

 

TIP: DO NOT dimension to line endpoints (except at the origin) as lines can be trimmed and the endpoints you selected disappear. Dimension from line-to-line rather than endpoint-to-endpoint. This is the key to sketch dimensioning.

Share this post


Link to post
Share on other sites
JD Mather

https://chronicle.autodesk.com/Main/Details/23894054-c11c-4f0b-9005-85c891bd69cb

 

Let's go pro.

Click on the link above and watch the video.

You can go directly into the arc command while in the line command.

Click and drag from the endpoint of a line (while in the line command) in the direction you want to go.

Then dimension the arc size and location and finally, drag the center of the arc to the construction line.

Share this post


Link to post
Share on other sites
JD Mather

Extrude Base.png

 

Extrude the sketch a distance of 30mm with a Taper of -7°.

Share this post


Link to post
Share on other sites
JD Mather

Corner Chamfers.png

 

Add 15mm Chamfers to the two outside vertical edges on the left side and 40mm Chamfers to the two vertical edges on the right side.

Share this post


Link to post
Share on other sites
JD Mather

Edge Fillets.jpg

 

Add 30mm Fillets to the vertical edges of the two 40mm Chamfers.

Share this post


Link to post
Share on other sites
JD Mather

Top Edge Chamfer.jpg

Add a 15mm Chamfer all the way around the top outside edges (be sure to click the top of the previous 15mm Chamfers).

Share this post


Link to post
Share on other sites
JD Mather

Dimension Visibility.png

 

Expand Extrusion1 and turn on the Visibility of Sketch1.

Right click on Sketch1 and uncheck the Dimension Visibility.

 

Start a New Sketch on the top face of the part.

Share this post


Link to post
Share on other sites
JD Mather

Sketch2.png

 

Project Geometry the centerpoint of the arc from Sketch1 as shown into Sketch2.

Sketch the Rectangle shown.

Share this post


Link to post
Share on other sites
JD Mather

Coincident Constraint.png

 

Add a Coincident Constraint between the projected center point and the midpoint of the left vertical line of the rectangle.

Share this post


Link to post
Share on other sites
JD Mather

Toggle Cetner Points.png

 

Window select the rectangle and toggle the line endpoints to Center Points.

 

Right click on Sketch1 and turn off the Visibility of Sketch1.

Finish Sketch2 and save the file.

Share this post


Link to post
Share on other sites
JD Mather

Dimension Rectangle.png

 

Dimension the rectangle as shown.

 

We have two extra Center Points (at the midpoint of the left vertical line and at the projected origin) that we don't really need and could toggle to Points, but there is no real need to do this.

Share this post


Link to post
Share on other sites
JD Mather

Hole Placement.png

 

Start the Hole command and hold the Ctrl key and unselect the two extra points as shown. Enter 18.5mm Through All as the parameters.

 

(Tip: If you missed this step and accidentally created the two extra holes - you could always right click to edit the feature and then Ctrl unselect the two extra centerpoints.)

Share this post


Link to post
Share on other sites
JD Mather

Shell.png

 

Turn the part over so that you are looking at the bottom.

Start the Shell command and click the bottom face of the part.

Set the Thickness to 10mm.

Share this post


Link to post
Share on other sites
JD Mather

Oops, I forgot a step. Delete the file and start over - right? NO!

Well the step I "forgot" should have been done before the Shell feature. Delete the Shell feature - right? NO!

 

Roll Up the EOP.png

 

Find the red End of Part marker (hereafter referred to as EOP) in the browser and drag it up above the Shell feature.

Share this post


Link to post
Share on other sites
JD Mather

CBore Hole.jpg

 

Start the Hole command and this time use the On Point placement option.

Click the Origin Center Point for the Point and the bottom face of the part to set the Direction.

 

Click the Counterbored Hole option and set the parameters as shown.

 

Drag the red EOP back down below the Shell feature.

Share this post


Link to post
Share on other sites
JD Mather

Project Edges.png

 

Turn the part over and start a new sketch on the top face.

Project Geometry the 4 edges as shown.

Share this post


Link to post
Share on other sites
JD Mather

Sketch circle.png

 

Sketch a circle from the hole center to the green snap point as indicated.

Share this post


Link to post
Share on other sites
JD Mather

Trim.png

 

Trim the circle and then Extrude 8mm.

Share this post


Link to post
Share on other sites
JD Mather

8mm fillet.png

 

Add an 8mm fillet around the top edge of the extruded cylindrical feature.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...