Design Help Carburetor Spacer Taper

[griffojYF22Y]

Hello, I am trying to create a carburetor spacer for a project I'm working on and I can't seem to figure out a proper way to make the taper and I was wondering if someone could help me out. The attached picture is what it should look like when machined.

[n_Sovljanski]

Hi,

I can suggest you to use loft command for one opening, then use mirror twice (horizontally and vertically). You can use circular pattern if openings makes square. 

[cadman777]

Looks not so simple.

A cone with a transition at top.

What are the dimensions?

Do you have any scan data?

[griffojYF22Y]

I can send you the Inventor file for the basic solid drawing minus the taper if that'll help you understand dimensions. Also, what do you mean by scan data?

[cadman777]

I'd like to see your inventor file, but I'm still using IV2010 so can't read newer files.

The dimensions I would want to see are various radial cross-sections of the ports.

Scan data is a pointcloud created using a laser scanner.

Here's an example.

You process the point cloud into a triangular or quad mesh.
Then you process that mesh into a surface or solid.
This requires very expensive hardware and software.

This is much more accurate then hand measurements.

Also you can use a CMM to get points, but you get them one at a time instead of a cloud of points.

The CMM's area also very expensive.

[JDMather]

Attach the *.ipt file of your attempt here.

[griffojYF22Y]

Here is the drawing I have, I'll send some pictures of an actual 2-inch spacer I have so y'all have a better idea of what needs to happen.

[griffojYF22Y]

 

 

 

 

 

[cadman777]

Thanx for the pics!

[cadman777]

Any chance you can post a STEP file?
I can't read your ipt with my old Inventor.

[griffojYF22Y]

When I get back to my personal computer I will convert for you.

[griffojYF22Y]

Carb Spacer File 

This was the only way I could send it. Hopefully, it works for you!

[cadman777]

OK. Got it. Thanx!

[JDMather]

Sketch1 is not fully defined and the Origin is not in a logical location?

What desired radius are these arcs?

[griffojYF22Y]

Both radii you pointed out are .875R/1.75" dia.

[cadman777]

That's what I meant when I said 'multiple sections through the bores'.

You need dimensions to get it right.

Anyway, find attached one way to do it, but it's a crazy mess. My basic assumption was the body is hogged out of a solid billet of aluminum, and the hollow cylindrical standoffs are welded in place.

I tried keeping it simple, but not knowing any of the dimensions except the flanges and o.s. body (from your STEP file), I really can't do justice to the model. Basically what I did was show you one way to do it. I first make a Loft cut for one bore and arrayed it 4 times. Then I trimmed back the center hump and contoured it. It didn't come out exactly right, but I didn't want to waste any more time on it. You would get the basic idea. Then I contoured the 4 mid-span protrusions as you can see in the model. Simple approach but what a mess of features. I'd like to see how others in here do it, maybe with less features and a simpler work-flow?

[griffojYF22Y]

So, some of the issue I was running into is that I don't have a set dimension for the internal radius of the "taper". It's more along the lines of "as long as the taper is smooth and flows down to the bottom of the bores it will work. I appreciate you spending time on this for me and helping me out. Thank you!

[cadman777]

You're welcome!

The way I've measured those kinds of things in the past before using laser scanning is to use paper or cardboard to cut a profile that matches the contour of the part. Or if they are standard radii, you can use a radius gauge on it to find the approximate radius. With the paper or cardboard, you can scan it into the computer using a multi-function printer and then bring that into Inventor as a pic file and trace around it. Or bring the scan into something like Inkscape or Gimp and convert it to a vector file (DXF), then bring it into Inventor. Then you can get your profiles close to what the customer's part is.

The problem w/the central hump in my part file is the sharp edges that warp up instead of transition smoothly to a tangency. I could do that with more time, but didn't think it was necessary, since you can 'play with it' to get it how you want. That thing took me around 3 hours to make, with a number of revisions, as you can see by the letter at the end of the file name. That's usually how it goes when I do surfacing like this part. In Rhino3D it probably would've taken me about an hour.

Incidentally, you will see which dimensions drive the design if you go into the sketches. I didn't take the usual time to identify them. But you can do that if you want. For example, the offset dimension in the bottom hole profiles is what changes the size of that hole. The hole currently is an ellipse of around 1" minimum radius as you can measure.

[Seymour-Butts]

Hopefully I've attached a model that should be helpful to you. I based the dimensions off of the Holly Carburetor website since they were close you yours. Your sketch was undefined making it very difficult to work with. My suggestion is to always fully define your sketches.... it will save you a lot of headaches down the road. 

You should be able to modify the "IntakeManifoldOpening" sketch. It defines Loft1. This should allow you to match the dimensions of the manifold you are planning to put this on. As you make changes to this sketch, you'll notice the connecting ribs change so play around to find what you like. Remember that when you are machining this, most of the internal radii will be generated by your tool diameter, so don't worry about trying to model them because they will come out smooth anyway. The model should be fairly flexible... meaning you should be able to make changes without causing problems. For example, you could change the thickness of the riser from 1" to just about anything and it should still solve.

You can add your own "light weight" features, as desired. I thought I'd point you in the direction of how I would generate the features you were interested in.

Let me know if you have questions. 

Cheers!

[johnsonshiue]

Hi Folks,

Sorry to join the party late! This is a very interesting challenge. To reverse-engineer the part, you will need to think about how it would be machined. A machined part should only consists of Extrude, Revolve, and Sweep. Other Freeform type of features like Loft, Boundary Patch, and TSpline cannot be machined easily.

Here is a 30-minute attempt. Enjoy!