Ports in a 4-valve head

[EngJW]

I wonder if someone could tell me the method that is used in making an intake or exhaust port. The approaches I have tried have failed. It must be possible, because there are many pictures around (even in the Soldworks start up screen).

I am trying to do this with lofting. There are a pair of round profiles in the combustion chamber and an oval profile on the side of the head. There is a path between them that makes a couple of jogs in different planes.

Every variation refuses to recognize the path. I tried making the path in 3d sketch view, and then with individual lines in different planes except I can't join the lines into a single path. I tried the piercing constaint between path and profiles.

Since I am new at this, if someone could suggest the methodology, I could come back with specific questions. Anything is appreciated.

Thanks
John Woodward

 

[TheTick]

Wouldn't this be revolve-able geometry?

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[EngJW]

It doesn't look like that would be it. The round profile needs to move along a curved path. The error keeps saying that the guide path does not pass through section 0, whatever section 0 means. I have the path connected (I think) to the center point of each profile. By the way, I can sweep an individual profile along the path, and the two profiles can be lofted together in a straight line as long as the path is not selected.

????

 

[EngJW]

Wow, that's discouraging. Actually, that thought has occurred to me but I didn't want to say anything since I am a beginner. I put a lot of hours into MDT5 and concluded that it was fine for simple constructions but could not do anything complex (that is, real world). Solidworks is much easier to work with, but now I am reaching the same conclusion.

I have many years of Autocad experience and I can layout some pretty complex designs in 2D, but with these solids programs I am spending too much time just trying to work around the system to get things to work.

I don't know how they arrive at all these nice pictures of engine designs such as seen in the SAE magazine, unless it is just marketing bull.

I really hope that I am wrong,

John Woodward

 

[sam53]

Have you tried lofting and then shelling the feature?

 

[djw2k3]

Hi John

Re, Your second post

AFAIK Guide curves need to intesect the sketched profile, not the centre points for lofting.

Some one please correct me if I am wrong

 

[EngJW]

Sam- yes, lofting and then shelling is what I want to do.

DJW- that might be my problem, although it isn't clear to my what is meant by intersecting the profile. If I have a circle for the profile, do I need to offset the guide curve from the center of the circle to its edge? Sounds cumbersome but I will try it.

Thanks

 

[EngJW]

After a few more hours of work-

Two separate round profiles will not follow their individual paths to a single oval profile.

One round profile will follow a path to the oval, but the result is not satisfactory.

I am forced to conclude at this time that Solidworks cannot be used to create merged intake and exhaust ports in an overhead cam engine. It could not be done with MDT5 either. At least with Autocad you can show in 2d what your intent is, and spend less time doing it.

 

[EdDanzer]

I think you can create the geometry. Try creating a 3D spline for the path, then a shape at each end of the path and loft. You will need to create reference planes and an axis for the valve at the start of the loft and planes to define the manifold connection location in relation to the block contact surface to finish of the spline path. If you want several shapes over the length of the port, just add more reference planes where you want the transitions. As to valve guide placement, that material and hole should be started from the reference planes and axis that is used as the start of the port and added after the basic port has been created.

 

[EngJW]

Ed- I think that is what I am trying to do but very likely I am missing the one small insignificant step that will make it work. I am at a disadvantage because I have no one here at work that I can ask. The other guys refuse to move beyond Autocad 14.

Cor- now that I have finished with my rant, I hope to wake up with another idea in the morning. I think I can make this work but I think it will be something less than what I really want.

Interesting comparison- at the last place I worked we tried to get Pro-E. They wanted something like $50 grand a seat with a special work station. I couldn't understand the work station (Sun?) concept, but then I am dumb about computers. They finally bought Ideas. Now I sit here with Solidworks on an old slug computer and it works ok.

John Woodward

 

[djw2k3]

Hi John,

Yes the guide curve must intersect the circle/profile edge. Well as far as I know anyway - what version of SW are you using?

 

[SBaugh]

Guide curves are the answer to your problem jlwoodward. Guide curves and possible more profiles. As the Loft twists and turns more profiles showing how the profiles changes "There are a pair of round profiles in the combustion chamber and an oval profile on the side of the head" The more profiles the smoother the transition.

Guide curves help connect these profiles together maintaining their relationship according to the way the guide curve is made and attached. With your guide curves I'm sure the 3Dsketch curve is going to be necessary.

IHTH - Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

 

[MElam]

If you only have 1 "path" like in a sweep, you should be able to use it in the loft while it is attached to the centerpoint.
In the loft command, select "Centerline Parameters" instead of "Guide Curves" and put your path in there. This option is meant to work like a path where the guide curves are meant to control individual vertices in the profiles.

 

[EngJW]

What I finally did was to make a single solid port by sweeping it, and then mirror it to make the two ports. Next, I used a cut sweep to hollow out the port and mirrored that also. Now the two ports are joined, although not with an oval shape that I wanted. There is a ridge along the line where they are joined, so I applied a fillet to the ridge.

The resulting port is good enough for now so that I can move on. I hope to come back to it after I get some more knowledge and experience. I probably need to learn more about making the guide curve and adding more profiles.

Thanks for all the tips.

 

[aamoroso]

Not sure if I get what you are saying, but if you draw a profile on top of a block and another on a side. Sketch on the right plane and give your self two seperate drive curve sketches, you should be able to Cut Loft from one profile to the other using both the curve sketches as guide curves. The trick is to make certain that the curve sketches are pierce mated to the profiles.

 

[Theophilus]

Finally read this thread.

Here is what I have done in the past--works very well. I have the same shape formed with a sweep (handle), except in positive form in a hand-held horn on my web site. Tricky at first, but not too hard to do with a sweep.

Here are some tips (not in this order necessarily):
1. Figure out the center of your path. This will be your "path".

2. Use an ellipse for your profile. An ellipse can be round where you need it to be, then morph into the oval you're looking for later when you need that form. This is controlled by your guide curves.

3. Your hole shape will be controlled by two guide curves. It sounds like your path will have a bend or two in it, but that this bend will at least be planar (I hope). If so, you will make one guide curve to govern the X axis of your ellipse and another guide curve to govern the Y axis of your ellipse. If you have a bend or two in your path, you may want to extrude a surface and then project one of your guide curves onto that surface to govern your X or Y axis in your ellipse.

Doing these things, you can form very complex geometry in a very stable way.

If this doesn't work, I'd be willing to look at your part and see if we can come up with a solution. I love this stuff.




Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[cpretty]

Correct me if I am wrong, but your main issue is with trying to do the 2 ports from the combustion chamber into one port exiting the head. From what I have read, you are trying to create this in a single loft. This will not work as the 2 separate sketch entities (circles) for the combustion chamber are not joined.

Your solution of creating 2 separate lofts for each port is correct. Creating a fillet to remove the sharp edge seems sensible, and from a realism point of veiw, it actually makes sense also.

With regards to other programs, I don't think anything else would handle 2 separate entities going into one in one single step.

 

[APPENG]

Just a side note and forgive me if someone has mentioned it (there are a lot of posts here) When i have to derive geometry of this nature I generally make them as a solid feature (multi-body solid) and hide the the cylinder head body or make it transparent. Then when I am satisfied with the shape and volume of the port(s) I use the combine feature to subtract them from the cylider head.

just a thought



Regards,
Jon
jgbena@yahoo.com