Solidworks question - editing a lofted feature

Big Train James

Western Thunderer
I'm in the midst of a 3d modeling project, to create a driver center for a PRR locomotive. I normally use Autocad for my cad work, including in 3d, because I've used it for a long time and am fairly fluent with it. However, I'm also in the midst of trying to learn Solidworks, so I'm trying to mimic my Autocad efforts in Solidworks with this driver center.

As noted in the attached video, I can handle quite a bit of the tasks in Solidworks, without incident. But I do have an issue when creating the wheel spokes. The problem I have is that the data I have on hand to create and loft profiles, results in too-short spokes which fully intersect neither the crank pin boss or the outer rim of the driver. So I need a way to lengthen them, without altering the overall characteristics of the orignal loft, meaning things like the rate of taper.

The solution is simple in Autocad, but maybe not so much in Solidworks. I've not been able to find a reference that tells me if I can apply my Autocad method to a Solidworks solution. Or if there even is a Solidworks solution. So I'm hoping somebody here can point me in the right direction.

It's all explained in the video, I believe. Much simpler than trying to describe the situation with words only. First though I have some images of the drawing. You can see the spoke profiles in the top right corner. Their positions relative to the wheel center and rim are called out as Section A-A and Section B-B, along the horizontal spoke to the right of the crank pin boss.
solidworks loft 001.jpg solidworks loft 002.jpg solidworks loft 003.jpg

And here's the video:

Hopefully someone can enlighten me.

Thanks,
Jim
 
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Big Train James

Western Thunderer
Not yet sure what the issue is. I've managed to include video previously, without incident. So it would seem odd to me that it's not working this time. Hopefully I can get it sorted out.
 

Spitfire2865

Western Thunderer
Where are your relevant planes for this loft? Solidworks only lofts between planes related to said loft profile.
According to the drawing, your spoke profile is determined at two points along the shaft, not its endpoints(which is reasonable from an engineering perspectove).
If your loft is only along this portion, it wont extend itself to the rim/boss. If instead you find a close enough approximation of the end of spoke at each extreme, you can have a loft of 4 shapes across the spoke profile. It wont be perfect but that should do it.

I am unsure if solidworks HAS a feature for extending a loft a set amount beyond the given references. Would be useful if it did though!
 

Big Train James

Western Thunderer
I presume the relevant planes would be same as for the profiles, as that's where I would have created them? That part isn't the challenge, rather it's extending the loft. I'd like to avoid the approximation of profiles at the rim and boss, if possible, if nothing else because when it comes to cad, I abhor approximations! :oops::rolleyes::cool: They make my eye twitch....

I am 100% in agreement with all sentiments expressed in your last paragraph :thumbs:.
 

Brian McKenzie

Western Thunderer
James,

An easy way to do what you need is to make use of some Surface tools. Turn on the Surfaces toolbar.

Use the Delete Face tool and select the end faces of your lofted spoke section (this action makes your spoke hollow).
Spoke_1.jpg


Then use the Extend Surface tool . . . . .
Spoke-2.jpg


. . . . by using these settings and specifying a distance.
Spoke_3.jpg


The spoke is still hollow, so use the Filled Surface tool and select the edge of one spoke end (you may need to turn off visibility of the rim or hub to pick it).
Spoke_4_Fill ends.jpg


You're doing well - so now repeat the Filled Surface action for the other end of the spoke :)


To turn the spoke back into a solid section, use the Knit tool

Spoke_Knit_5.jpg

Done!

-Brian McK.
 

Big Train James

Western Thunderer
Thanks Brian! I'll have a go at it tonight. I've never done much with surfaces other than to use them as slicing shapes. It's probably mostly down to the issue that I seem to end up with non-watertight entities that I can't manage to turn back into solids. Plus I normally can accomplish most of what I need with solids.

It's also interesting that in Solidworks, the extending function works for surfaces but not solids, whereas in Autocad it appears to be the other way around.

Thanks again, I'll post results when I have them.
Jim
 

Brian McKenzie

Western Thunderer
. . . . I seem to end up with non-watertight entities that I can't manage to turn back into solids.

Sometimes SolidWorks fails to Knit if too many items are selected at once, but by using a second application with fewer parts selected each time, it gets there.

The trickiest part of shaping driving wheels is the blending and flaring of spokes into both crank bosses and counterweights - where they intersect at other than 90 degrees. You won't be satisfied with simple fillets ;)
 

Big Train James

Western Thunderer
Success! Following the steps Brian outlined, I was able to extend the spoke. I had some issues along the way, namely that the edges at the rim end of the spoke are not co-planar following the the surface extension. And also there was that tiny overlooked step of clicking the "create solid" box when trying to knit everything back together :oops::rolleyes::confused:. But in the end, everything has apparently turned out correctly.

loft fix test.JPG

Now that I have this figured out, I'd like to hear more about the process used to blend the spokes into the crank pin boss and rim. There are a lot of compound curves to consider, so I was planning on utilizing the variable fillet functionality in Solidworks (Autocad doesn't do variable fillets, which is one of the more disappointing things about my experience with it). Is there another process that I should pursue? I wouldn't be surprised to learn that I will need to do some more lofting and so on to achieve proper results. Hoping for the best, I don't have any more hair to pull out.

Thanks again to Brian for the solution. I now know more than the instructor that is teaching my Solidworks class :eek::(:cool:. I'm sure more questions will follow.

Cheers,
Jim
 

Brian McKenzie

Western Thunderer
I had some issues along the way, namely that the edges at the rim end of the spoke are not co-planar following the surface extension.

Extend both ends of the first spoke by utilising dimensions that buries it deeply into both the rim and into the contoured shape of the crank boss (I prefer this to using the option of "Up to Surface"). Then, when after having created an Array of spokes, use the Combine tool to merge all spokes, crank boss and rim as one, and the excess overlapping internally [:confused:] gets trimmed away automatically.

I'd like to hear more about the process used to blend the spokes into the crank pin boss and rim.

Variable Fillet works to some extent, but more shaping of the spoke where it meets the crank boss is often required. For me, this tends to become a bodge of assorted surfacing tool functions, lofts and fillets.
Best I can advise is to study this brilliant video tutorial:

Cheers, Brian McK.
 

Big Train James

Western Thunderer
Thanks for that link Brian. I watched part of the presentation last night. Went to bed feeling both inspired and somewhat demoralized. I now feel utterly inadequate with respect to 3d modeling, when I thought before that I was decent at it :(.

I'll watch the rest this weekend. Then I guess I have some exploring to do in both Solidworks and Autocad.
Jim
 
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