Create a work plane at a point along a curve? Help?!

[kingneptune117]

Hey all,

 

I'm a bit of a noobie here. I have been using inventor for a while on and off as a student, and I finally got a job where I need to use it for some things. For practice I decided to draw up the desk lamp that is next to me. Anyways, I need to create a work plane at the place that I've shown in the attached image. This is so I can place a hole where the cables and what not go into.

 

I have no idea how to create a plane that is tangent to the point on the curve that I want. It's really bothering me

 

My sketch is fully constrained. I have attached my IPT and an image for visual aid. Thank you.

Dome.ipt

[kencaz]

Easier way may be just create an angled work plane off your original plane and extrude cut...

 

[JD Mather]

kencaz might have answered your question,

but it is important to know how to create a workplane at ANY surface pierce point, so I am going to explain a trick (and other problems with you part).

 

Create sketch line to define pierce point on face.

Start the Workplane command, but - (this is the trick)

Right click and select Create Point and then select the line and the face - Inventor will find the pierce point intersection and create a workpoint.

Now select the workpoint. (this could also be done in two steps rather than using the right click trick)

 

[JD Mather]

Now for your "design".

 

Sketch1 looks like you used the Autodimension tool rather than do YOUR work.

The result is dimensions that cannot be inspected and therefore a part that cannot be manufactured to specifications.

 

Also the right side line (in image attached) is not vertical. Is this really really really what you want? Tell me the angle of that line?

 

[JD Mather]

Now edit Sketch2

right click and select Show All Constraints.

Is this what you really really really want? All of these constraints are going to make your file size larger than needed and start to bog down your assembly.

 

Pattern Features rather than Sketches whenever possible.

... and your sketch wasn't fully constrained.

 

 

Also, Workplane1 is a duplication of the YZ plane and therefore obviously not needed.

 

I recommend you go through this document http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

[JD Mather]

Now go to the Left side view on the View Cube and examine the slots.

Is this what you really really really want?

 

[Pablo Ferral]

Listen to JD - he knows his stuff

[kingneptune117]

kencaz might have answered your question,

but it is important to know how to create a workplane at ANY surface pierce point, so I am going to explain a trick (and other problems with you part).

 

Create sketch line to define pierce point on face.

Start the Workplane command, but - (this is the trick)

Right click and select Create Point and then select the line and the face - Inventor will find the pierce point intersection and create a workpoint.

Now select the workpoint. (this could also be done in two steps rather than using the right click trick)

 

[ATTACH=CONFIG]43328[/ATTACH]

 

JD, thanks for all the help. However, when you say "create sketch line", do I create that line in sketch 1? or sketch 2? Or is there some other way to create a sketch line in the 3D view? Thanks.

[JD Mather]

In Sketch1 or any new sketch.

[kingneptune117]

In Sketch1 or any new sketch.

 

JD, if I open sketch 1, draw a line that intersects the shape where I want it to, and click finish sketch, my view returns back to 3D. Will the 2D line that I just drew in sketch 1 still be visible? if not now am I supposed to click on it to form the point for the plane? Sorry for the trouble but I really want to get this right.

 

Maybe you meant use the 3D sketch tool to draw a line in 3D?

[JD Mather]

No, I did not mean the 3D sketch tool.

Expand the Revolve feature in the browser.

Right click on Sketch1 and select Visibility.

You can now see the sketch at any time and turn on/off visibility as required.

This should have been covered in your class.

[kingneptune117]

Gotcha. And I only ever took one class on it in high school. I am now a junior in college however I use inventor for some class projects but I have not had to create a work plane on a cylindrical surface (or is it just a curved surface?) until now.

[ecshclark]

I think your question to create a plane tangent to the surface through point was skipped.

 

In the Browser, select Sketch1 under the Revolution1 feature, right click and toggle the sketch visibility on.

 

Next, in the Work Features tab, In the pull down menu under Plane, select Tangent to Surface through Point. Select the outer surface of the lamp, then select the point in the visible Revolution1 sketch. You will now have a work plane tangent to the surface at that point.

 

Create a 2D Sketch on the work plane, then use Project Geometry and select the point from the Revolution1 sketch. Draw and constrain geometry to this point needed with your feature. Or select finish sketch and use the projected point to cut a hole using the Hole feature command under the Modify Tab in he Ribbon.

 

When finished you can go back and toggle the Revolution1 sketch visibility off.

[ecshclark]

Sorry, I see JD did explain create the plane just before I did!

[kingneptune117]

Ok, I finally got it. I'm not sure if I did it the exact same way you are referencing. I opened up sketch one, placed a point where I wanted my plane, finished sketch, the in the 3D model I turned on the sketch visiblity and used the "Plane tangent to surface through point" command to make my plane where I wanted it.

 

However, the only problem I have with this is that I can only make my plane where the original 2D sketch lines are on my 3D model. I tried dragging the point somewhere else on the 3D model, but it only drags along the line (obviously). What if I wanted to place my plane, say, here (shown in the image)?

[JD Mather]

Same way you created the other workplane.