trouble projecting geometry with 2009

[Harley157]

I have a round pipe that is a 3D solid. I want to project an L shaped

mill cut on one end,180degrees apart in sketch mode. I cannot seem to project this geometry onto the cylindrical pipe using workplane. Would anyone have any suggestions. I could send the drawing if you need to look at

it. Thanks in advance.

[JD Mather]

Attach the file.

3D sketch

Include geometry (2d sketch)

You can now project

 

or

Emboss

 

I doubt these methods will give what you really want. I'm assuming the slot an end mill would cut as the tube is translated/rotated.

[shift1313]

JD, do you have to include geometry in order to project? I project onto surfaces in 3d and i never have to select Include Geometry first.

[JD Mather]

JD, do you have to include geometry in order to project? I project onto surfaces in 3d and i never have to select Include Geometry first.

 

Good catch. I didn't have Inventor in front of me and was going from (faulty) memory.

[Harley157]

Yes, the 2d sketch slot geometry would wrap a little around bottom. I had thought that once I projected the geometry, I could then do a cut-extrude. Maybe this the wrong approach. If there is a better way, I'm all ears. Thanks.

[JD Mather]

Attach what you have so far.

[Harley157]

Send me your email and I will send the IPT file. I noticed it wasn't listed in the files for attachment. You can then open it exactly the way it looks. Thanks. I have it ready when you are. It should show

you what I'm trying to do, which really isn't that much. Just need

expert advise on dealing with it. I may be using a completely different

approach. We'll see.

[JD Mather]

I noticed it wasn't listed in the files for attachment.

 

I don't know what this means. Open the file. You should see a red End of Part marker in the feature history tree browser. Drag this EOP marker to the top of the browser hiding all features. Save the file.

 

In Windows Explorer right click on the file name and select Send to Compressed (zipped) Folder and then attach the resulting *.zip file here.

[shift1313]

as far as i know you cannot extrude a 3d sketch. You will have to sweep or loft it. can you post a screen shot as well?

[Harley157]

hone housing.zip

 

Here it is, I hope.

[shift1313]

are you cutting through to the center? as a latching mechanism? or do you truely need to mill this profile offset from the surface?

[shift1313]

At work i only have IV11 so i cant open your file but the zip did work. Depending on how you want to make this cut there are a few options. if you draw your 2d sketch off the surface, start a 3dsketch and project geometry to the outside face of your tube and the inside face of your tube you can use them for lofting curves. This may be the easiest option. You can also take the projected curves, make a boundary surface and thicken/cut with it. You could also sweep the projected curves if you make a path.

 

If the image below is what you want you could just extrude the 2d sketch but hopefully the procedure will show you an option. If you can fill me in with a little more detail on what you want to do i may be able to help more.

[Harley157]

The mill cut just cuts through the side wall. It is a latch for another piece with 2 ears to lock it in. It basically slides in and then twists to lock. This is close to what I wanted. The slot should be .350 wide on cuts. It is a little wide in the image here. I'm still not 100% sure how you did

this. I had the geometry on a workplane. Is it not possible to project to the surface of 3D model? Your method seems to work, just not real sure how you did it.

[shift1313]

will this be done on a 3axis machine or will you have a 4th axis? If it plunges through and its a 3axis operation i would just extrude your 2d sketch. if this is a 4axis operation there are some options when projecting geometry. apply to closest point comes to mind.

[Harley157]

Yes, this could be done 3 or 4 axis. Probably 4th axis to get the curved cut.

[shift1313]

well there is another option as well. You could do this in two sketches. One would be a revolve operation and one an extrude operation. This would simulate your mill bit going in from the edge, and the revolve would be the rotary axis turning. You would have to go back and fillet the inside edges to your spec. I dont think inventor has this feature but i know SolidWorks has a sweep cut. Essentially you would draw your mill bit and the path and it would remove the material.

 

Later tonight ill think about it some more.

[JD Mather]

I think maybe you are making this one a bit too difficult. No 3D sketch needed.

 

BTW the equivalent to SWx method (sort of) would be to do a Sweep Cut with Guide surface.

[JD Mather]

After thinking about it I just realized I could simplify it even further removing the two user workplanes.

 

Simplified Sketch2

Deleted Workplanes 1 & 2 and Sketch3

 

60° angle can be set to any desired angle of rotation for the slot.

Extrude pie shape and trimmed lower rectangle midplane width of slot.

Extrude lower trimmed rectangle through all.

Revolve upper angled rectangle.

Add Fillet in lower corner.

 

Let me know if you can't figure it out and I'll walk you through it step-by-step.

[Harley157]

Seems to be many approaches to this. JD and Matt have gotten results

with different methods. The only other thing for finishing this is the milled

cut in on the opposite side too. This cut going down instead of up. Two ears

with lock into these and unlock with a twist motion.

JD, I would like to see your simplied version step by step. I'm extremely

interested in how you accomplished this. I really never thought about using

the revolve command in 2D sketch mode. Interesting. I just thought I could

create the milled-cut, 2D geometry and then project it onto the 3D solid and cut-extrude the opening. I definitely am overlooking other possibilities here. Thanks to both of you.

[shift1313]

thats kinda what i was thinking jd. I did what you did with a revolve "tube" that extended past the origin point and a sketch on the xz plane in my case. My sketch is a little different than yours.

 

Harley i drew a rectangle offset from the center point(width of your mill bit) Then i drew a line from the center point up 60degrees and connected the center lines with an arc. Making sure to dimension all your stuff. I did an extrude of the rectangle bi-directionally(1" in my case), then a separate extrude of the triangle back .5". Fillet then do a circular pattern around the Yaxis for the second slot.