extruding a vertical rib

[Art K]

Working on the same bellhousing. The last portion I'm having trouble on is the two vertical ribs. I have tried to use the wrap, project. I can't make it work. Any suggestions? I drew the ribs in the location where they should project. The ribs radius is 2.276 .047 higher than the 2.229 radius of the body of the bellhousing.
Art

 

[Old Geeser]

Art, I did a extrude "to geometry" feature and got ribs to the bellhousing. Is this what you are trying to do, or do I not understand?
Karl

 

[Old Geeser]

like this?

 

[HaroldL]

I drew the ribs in the location where they should project. The ribs radius is 2.276 .047 higher than the 2.229 radius of the body of the bellhousing.

Art, The extrude type "To Next" will only work with a single loop sketch. For this instance I converted one rib sketch to Reference geometry, extrude the remaining sketch To Next, then Mirrored that to the other side using the YZ plane as the mirror plane. Sometimes, if the part is symmetrical, you can make use of the Mirror function to make your sketches simpler.

I might caution you to use fully constrained sketches, even when just fleshing out a design. It makes in a whole lot easier to trouble shoot sketches and features when something goes wrong. And if you need to make minor tweaks you have dimensions to work with.

Here's a snap shot of how I constrained the sketch of the rib.


And here's the model:

 

[Art K]

Albie And Harold,
That isn't quite what I wanted otherwise I think I'd have figured that out. "The ribs radius is 2.276 or .047 higher than the 2.229 radius of the body of the bellhousing". Harold the portion of the drawing you have in yellow is the 2.229 the rib is .047 taller than the 2.229 and is at a 2.276 radius from the same center point as the 2.229 radius. that is why I was trying to wrap project it to the 2.229 surface. It does make sence to do one side and mirror it but its been a long day and I'm about to get horizontal. Harold are there tutorial videos about using constraints? My only training in CAD was in Master Cam about 15 years ago at tech school. and I don't remember anything about constraints, or when to use them.
Art

 

[HaroldL]

Maybe you could post a screen shot of the finished rib. The only thing I did was to apply constraints and add some dimensions. As yo can see there is a 2.276 radius dimension on the arc end of the sketch. I thought I was interpreting your comments correctly, if you had something else in mind let me know

Harold are there tutorial videos about using constraints? My only training in CAD was in Master Cam about 15 years ago at tech school. and I don't remember anything about constraints, or when to use them.
Art

There is a whole suite of tutorials located on the Alibre Home page, and if you do an internet search on Alibre Tutorials you'll find a lot more on various subjects.

 

[Art K]

Harold,
Sorry bout this is the closest to a screen shot I can do. If I was capable of doing a screen shot I wouldnt have needed help. I bought the blueprints for George B's flathead V8 and decided the bellhousing was a good place to start.
Art

 

[HaroldL]

Now I understand, the rib is raised .047 above, and along, the curve of the bell. That is possible with a sweep feature from the flange To Geometry of the square boss, then mirrored.

 

[Art K]

Harold,
Thanks for you help. But I am not following this completely. I was looking for drawing 15 and 16 which the sweep refers to. I extrapolated where 15 is on the mounting flange but I cant figure out where 16 is.
Art

 

[HaroldL]

Here's a short video that should explain how I accomplished the sweep.

Rib Description.mp4

Shared from Screencast.com

www.screencast.com

 

[Art K]

Harold,
Thanks, after watching the video everything made total sense. I will have a go at it tomorrow.
Art

 

[HaroldL]

Glad to help out. Good luck on the rest of the model.

 

[Art K]

Harold,
I watched the video and it made sense till I got home and tried to do it. Probably doesn't help I've been sick with cold symptoms, tested negative for covid. One thing I noticed is my face for the "to geometry" is face 68 not 73 like yours. I can't seem to make the project to sketch function work. If I try to get sketch 16 by activate sketch Y Z axes then click on the 2.229 radius I then get a 9003 error sketch can't be used because an endpoint is wrongly shared by multiple primitives or overlapped figures.
Art

 

[HaroldL]

It sounds like you're having trouble creating the Path by using Project to sketch. Here's another vid with more explanation on creating the sketches.

Further Explanation of Sweep.mp4

Shared from Screencast.com

www.screencast.com

Let me know if it makes it any more clear.

 

[Art K]

Harold,
I tried to follow your video, it was clear after all. But no joy. I was not given an error message when I punched in the info in the sweep window it just did nothing. It didn't highlight the box to apply nothing. I even reduced the size of the drawing from .209 to .176 as you have what have I got wrong?
Art

 

[HaroldL]

@Art K , for a sanity check, edit each sketch and run the Analysis tool just to make sure they are okay.



If that doesn't show up anything can you package and upload the model you're having the problem with?

 

[Art K]

Harold,
Ok I am up to my ears in frustration. I checked the drawing and it had open loops no healing option. I put a radius on each corner still open loop. Deleted and redraw fine.
Previously had open loops No problem. go to project to sketch to create drawing 15 then model this time analyze overlap. I will be looking on to see what you have figured out but will be out of town for the holidays. Thanks for your help.
Art

 

[HaroldL]

Looking at the profile sketch were a couple of extra sketch figures that aren't needed. After deleting them the rib sweep completed but needed a different stopping face.
I detailed it in this video.

Rib Analysis.mp4

Shared from Screencast.com

www.screencast.com

And here is the model with corrected sketch.

 

[Art K]

Harold,
I was on vacation the week between Christmas and new years. I watched your video but had no computer CAD capable. I have worked on it this week especially this weekend. But there is no joy in Mudville. I did change some things in sketch 14, like the Collinear face. Ended up with no errors when analyzed. On sketch15 with the project to sketch there was an open loop error but your model had that as well so I figured it must be ok. I don't understand what is wrong.
Art

 

[HaroldL]

Hi Art, I analyzed your sketches and they check out okay. The sweep works fine with your Profile and Path sketches as you have them created. I set the Sweep Type to "To Geometry" and selected the inside face of the rectangular boss as the Geometry Target, it's highlighted in the screen shot.

The Path can be an open loop, the Profile you are sweeping must be a closed loop. Just make sure you are selecting the right sketch for each function, if they are selected in error the sweep will not work - Sketch<14> is the Sketch to Sweep and Sketch<15> is the Path Object. It may help if you rename then according to their intended use.




Another option for the To Geometry target is the front face of the rectangular boss and add a negative offset (-.156) so the sweep completely intersects the fillet.