[skippy]

I started learning SW some months ago and have got quite comfortable with it (love the parametric aspect) and thought I'd start drawing a cylinder head (DOHC 4 valve). All was going well until I got to the intake and exhaust ports. I've just spent 3 straight days of agony trying to do one intake port but can't manage it. I previously drew this engine up in Rhino 5.0 (I was really proud of how the port surfaces turned out in Rhino) but rather than try to import it, I just started again from scratch. My method was to sketch the cross section of all required items (ports, spark plug, cams, buckets, etc..) on a plane that runs across the middle of cyl 1. There are 2 (intake) valves that are either side of cyl 1 plane and their respective runners join together into one opening on the port face (side of head) so I made a plane on the required angle. Here’s where things went wrong in several areas and I’ve spent plenty of time on Google and YouTube prior to asking for help here.

(1) Getting the cross sectional sketch of the port from cyl1 plane to cyl1 angled plane, as it seems in SW you can’t project a sketch to an angled plane like you can in Rhino. (you can but it doesn’t produce the required results. See Temp3.SLDPRT) I tried drawing the sketch in 3D sketch but it was nowhere near what I wanted and even worse was trying to draw the circles (for loft/boundary) when the guide line isn't in the usual XYZ planes.

(2) I tried Loft and Boundary Cuts many many times and even after adjusting the points I always end up with a poor quality surface (wrinkles causes by self-intersections in the cut even though the reference geometry (guides) are just simple slow splines. Funny thing is that I tried it now (Temp4.SLDPRT) (even though it’s a loft rather than a loft or boundary CUT but doubt that affects things) and it looks quite acceptable so I think the problem must be my poor quality loft/boundary references, i.e. the 3D sketch based off the guides produced in the sketch on the angled plane.

I’ll be happy just to receive some pointers on this one but just in case someone wants to have a go at the real thing, I've included a much cut down version of the original file. (I got rid of all the warnings I could that had resulted from removing the majority of the sketches and features (valves, plugs, other cylinders, etc.) from that file but a few still remain.)
Cheers

EDIT: Please find the attachments further on in later post.

[Mike 1948]

I tried to open the files but always get "unexpected error" and won't load.
Have you tried to Copy and then paste the sketch onto the angled plane?

Mike

[budgieW]

Solidworks it a little shy on surfacing tools, you may need to look at something with a little more grunt, NX, CREO or CATIA

[skippy]

As pointed out by Mike, Temp1 had some errors so I re-did it (attached here) as Temp1a.

Temp1b (attached here) Someone elsewhere suggested that if you get a sketch on a regular plane and the extrude it through the angled plane then convert entities on an angled plane sketch you can get the correct shape. It didn’t work for me as shown here. Maybe however, I am not doing it correctly.

Temp4 (yesterday’s files) is a loft which went ok

Temp3 (yesterday’s files) shows how things skew when you convert entities from a regular plane to an angled plane.

Temp2 (yesterday’s files) … I no longer remember what that was supposed to show.

Budgie, I certainly agree that Catia and NX, etc. will do a better job of surfacing but unfortunately they are out of the question for me.

Mike: "Have you tried to Copy and then paste the sketch onto the angled plane?"

Hmm.. now that I think about this I think the whole angled plane thing is not what I need because if (a) I did the type of projection I was looking for onto an angled plane (like Rhino can do, i.e. looks exactly the same (position and placement) when viewed normal to the original plane) then this isn't going to help me as the X size valve throat will actually be a bigger diameter than that in its real size on the angled plane. Possibly I could use this on the port centerline only as it's just a guide. (b) If I do the sort of projection that SW does to an angled plane the positioning ends up skewed. That took a bit of explaining and I wouldn't be surprised if you couldn't follow me.

I'm convinced a 3D sketch is the way to go to get my Loft or Boundary cut references. As mentioned yesterday, what I found challenging to impossible is to get guide circles on a spline so that they are normal to that point in the spline. If I don't use circles (along the spline) as guides, the loft/boundary feature loses diameter in that area. Then again, maybe I should just do a start and finish circle at each end of the spline and use guide rails (inside outside and or centre) for the loft/boundary feature.

One more thing. Looking at what I am trying to do, would those of you who are knowledgeable in this area, be inclined to do a loft or boundary feature for the full length of the port or would you do a loft only along the spline and use revolved cut for the top and bottom ends seeing as they are concentric? (revolved cut ends up with a perfect cut).

EDIT: Please find the attachments in next post.

[snowyskiesau]

Unrar gives an error message and the resulting extracted files can't be opened in Solidworks..

[skippy]

Try this.

[skippy]

Ok, here's one (Temp3a) that illustrates the problems in a better way complete with annotations on each sketch. This one shows what happens when you (a) convert entities to an angled plane (valve throat ends up far away [in engineering terms]) (b) paste to an angled plane (angles and positioning are off).

Unless someone happens to come up with a better idea, I'm now inclining more towards making revolved cuts at the valve throat and the top parts of the port as both would be concentric cuts, then try to make 3 splines (center, inside and outside of port) connecting the 2 revolved cuts in order to use as guides to do a boundary or loft cut that will hopefully join both revolved cuts thus making one complete port.

Another possibility: Seeing as the whole port from top to bottom is mathematically defineable and not overly complex, I've even wondered whether I should draw it all up in Rhino and import it.... As I mentioned earlier, Rhino is brilliant for surfacing. I've never done an import from Rhino to SW and I have no idea how good the translation would be nor how difficult it is to do it but there are a few tutorials on YouTube about it. Food for thought...

[hanermo]

Not related to SW, but..
Iges or STP files import and export well to from Rhino.

Make your assy from multiple parts.
These parts reference individual files.

These are called instances, and done with the place command in Rhino.

It will likely work, and you only need to do the difficult bits in Rhino if you wish.

[skippy]

Not related to SW, but.. Iges or STP files import and export well to from Rhino..

Do you know which is better for surfaces, IGES or STP?

"Make your assy from multiple parts. These parts reference individual files. These are called instances, and done with the place command in Rhino. It will likely work, and you only need to do the difficult bits in Rhino."
I don't quite follow you here. Are you saying to make the whole assy in Rhino using "instances" and the place command OR just do the difficult bits in Rhino (i.e. ports) then import them (the port surfaces) into my SW head casting drawing (head.SLDPRT) and hopefully fuse the 2 together?

I CAN'T EDIT EARLIER POSTS BUT JUST TO LET YOU KNOW THAT EARLIER FILES I UPLOADED CAN'T BE READ. HOPEFULLY TEMPSW.ZIP LOCATED FURTHER ON CAN BE READ.

[alexhawker]

Use a derived sketch.


Sent from my iPhone using Tapatalk

[Mike 1948]

I tried to open the new files in SWX 2013 and 2014 but still could not open. I get "unexpected error". Also, if you import the part or pieces into SWX they will come in as a "dumb" solid and you will not be able to modify them. You can add to or subtract from, but not change size of features.
Good Luck
Mike

[Coetzee]

What version of solid works are you using? I can't open these files still. I've got access to 2012 and 2015.

[skippy]

Use a derived sketch.


Sent from my iPhone using Tapatalk

Derived sketch, while being very handy, will place a sketch on the angled plane in the same way as copy/paste but won't do what I need in this case. The Temp3a file explains why but at this stage no one can open it. Grrrrr.

[adamw]

Go to grabcad.com, search "cylinder head". There are some very nicely done 4 valve cylinder heads on there that you can download and look through how they have been modelled. I haven't done a 4 valve port but on the 2 valve head I modelled I done most of the general port shape with lofts, then added details like the valve guide boss as separate features.

[skippy]

Good suggestion Adam.

[skippy]

I'm wondering if the problem is the online zip converter I used to zip the files (cnczone won't accept SW files) because now that I think about it, I shared a file with a mate of mine some weeks ago and he had no problem. I've now re-zipped the files using the standard Windows zip function and here they are. Could someone try to open one of the files (X64 2015) please and let me know if it works?

[skippy]

Well, I finally got it sorted. It's another very late night so I haven't got time to post a sample of the results now but will do at the first opportunity. I needed to watch a few youtube videos on sketch planes in 3D sketches. Once I saw someone doing 3D sketches on all sorts of angles using non-regular planes within the 3D sketches it all clicked for me. :banana:

I'd still appreciate it if someone could let me know if they can open any of the above files now that I have re-zipped them another way. Thanks for your suggestions. I'll repost in the next day or so.

The second video is relevant from 12:30 onwards.

https://youtu.be/BqPZAuTfYeE

https://youtu.be/lHxMuE3vWlE

[Coetzee]

I don't know if this is what you wanted, but I got this shape using 4 separate surface lofts and no guide curves.
Attachment 284056

I generally avoid using 3d sketches because they're a bear to define properly.

Anyway, once you have the surface lofts right, you can do a surface knit, then a thicken to get the solid geometry.

[skippy]

I don't know if this is what you wanted, but I got this shape using 4 separate surface lofts and no guide curves.
Attachment 284056

I generally avoid using 3d sketches because they're a bear to define properly.

Anyway, once you have the surface lofts right, you can do a surface knit, then a thicken to get the solid geometry.

Absolutely that's what I wanted and thank you very much for your input. I'd be embarrassed to tell you how many hours I spent trying to get this right this week and finally gave up out of disgust on Friday night for the very reasons you state (3D sketches are a bear to define) plus I had major problems getting entities (that came from Convert Entities) to select for a loft/boundary cut, then having to repair them many times over.

One thing I have learned in this exercise is that I should never have started this as a 4 cylinder engine but should have started as a one cylinder then when everything is as I want it, just multiply it out across the cylinders. Would have saved myself lots of work in both deleting when something doesn't work and multiply when hoping it does work (but didn't).

Once again thanks

[Coetzee]

Absolutely that's what I wanted and thank you very much for your input. I'd be embarrassed to tell you how many hours I spent trying to get this right this week and finally gave up out of disgust on Friday night for the very reasons you state (3D sketches are a bear to define) plus I had major problems getting entities (that came from Convert Entities) to select for a loft/boundary cut, then having to repair them many times over.

One thing I have learned in this exercise is that I should never have started this as a 4 cylinder engine but should have started as a one cylinder then when everything is as I want it, just multiply it out across the cylinders. Would have saved myself lots of work in both deleting when something doesn't work and multiply when hoping it does work (but didn't).

Once again thanks

If you tell me what version of Solidworks you have I'd be happy to send you this file so you can look at the steps. (Newer versions of Solidworks cannot save old versions files so it's very important to always state what version you are using if you are sharing files and want help).
In my opinion the best way to do this model is to make a 2d sketch that contains the overall dimensions of the part and the tube diameters at each change or bend. Then to do one 3d sketch with circles at each of those points. Do surface lofts. Do a knit. Do surface fillets between each joint where necessary. Then do a thicken operation on the final surface.

Solidworks has a lot of quirks. A really good way to learn is to get on grabcad, download models made by people who seem to have had a job before, and drag the blue bar at the bottom of the feature tree through the model from start to finish.