Had Another Go

[David JuppParticipant @davidjupp51506]

NO – as I’ve now said twice in above posts, the path and profile sketches do not have to meet/contact.

It generally makes more sense if they do, even if just for an ‘understandability’.

Jason’s latest screenshot clearly shows the sweep working when the sketches are some distance away form each other.

 

If in doubt, just try it anyway.  Nothing lost if it doesn’t work, and the error message may help you to work out what needs to be done to fix it.

If it works, but gives a result you didn’t expect, you will probably learn something – or at least have a specific question to ask.

[JasonBModerator @jasonb]

Right I have got Nigels file and this is one way to proceed.

 

 

Open the file

Right click on the red “sweep” in the tree on the left and click delete.

Right click “sketch 1” also in the tree on the left.

Now your icons are a bit different to mine but you should have similar. First click “select all” which will make everything on the 2D sketch go blue.

Then click “copy”

Then Click “Deactivate Sketch”

Click ignor to the warning.

 

 

Now click the “ZX Plane” probably easiest from the list on the left

Click activate 2D sketch

Click “paste” and that will put the sketch you just copied onto the screen

Click “deactivate sketch”

 

 

Now you can do the sweep by Clicking the “sweep” tab at the top

It may well automatically put sketch two in the “sketch to sweep box” if not click that box and then the sketch either from list or screen

Click the path box and again select what is now “Sketch 3” from list or screen

If all is well you will then have your chassis so click OK at the bottom of the sweep box.

Video is just uploading

 

Another option would be to just delete the red “sweep” , select ZX plane and redraw the guide lines then use that in a new sweep.

[JasonBModerator @jasonb]

[Nigel Graham 2]

On Nigel Graham 2 Said:

Mmm. I didn’t think it would even be swept because I thought the right part of the section has to meet the start of the guide-line, as well as being the right way round of course.

My reason for saying it was important to set them both at 300mm or half chassis width in your case was to make it easier as it saves having to workout offsets you just need the width between the rails front and back. Also it make sit easy to mirror the other chassis rail if you have set the first the correct distance from the ctr line. And going forwards you will have a chassis that is symmetrical so other parts and be assembled easily on that same ctr  linelike the boiler.

For a one off sweep it is not a requirement that they touch

[Nigel Graham 2]

On Nigel Graham 2 Said:

Mmm. I didn’t think it would even be swept because I thought the right part of the section has to meet the start of the guide-line, as well as being the right way round of course.

Any demonstration or exercise should be designed to work first time; so while the sweep is possible when they don’t touch, it’s more likely to do what you expect if they do. Especially when the path has been deliberately offset from what will become the chassis centre line so that the opposite rail can be mirrored from the first. That’s not advanced but a basic technique that ought to be learnt from the start to save time, effort, thinking and potential cockups.

I turn off the visibility of planes, grid and axes(and any snaps to them) because they’re only useful when beginning a sketch; once it’s started it’s more helpful to think about top, bottom, sides, centre etc of the object instead of abstract construction geometry.

As an aside, to me these rails with the ‘C’ on the outside look odd. Everything I’ve worked on them has it on the inside, with the crossmembers notched to them:

[JasonBModerator @jasonb]

So following on from that I’m sure Nigel and everyone else spotted that the sweep does not actually follow the guide which was the correct 6″ from ctr line at the front and 7.25″ at the rear. So lets correct that.

 

Right click “sketch 2” and select “edit”

As you had copied the C section it comes without dimensions so rather add them for overall width and the thickness of the web. Then when you enter half chassis width of 6″ from the centre line the whole thing will move.

Deactivate sketch and the swept profile is now in th eright place.

Generate to last and save.

[Nick Wheeler]

On Nick Wheeler Said:

As an aside, to me these rails with the ‘C’ on the outside look odd. Everything I’ve worked on them has it on the inside, with the crossmembers notched to them:

 

Well Nigel is in good company as the likes of Foden and Clayton & Shuttleworth both had the rails flanges outwards as did the Hindley

[Nigel Graham 2Participant @nigelgraham2]

Nick –

That outwards-facing arrangement of the channels seems to have been quite common on early road vehicles, as Jason points out, and I think on some railway rolling-stock designs. It probably facilitated construction by brackets and bolts or rivets, because the connectors then all work on flat faces with no need to cut frame-members to fit inside the profiles.

 

Thankyou Jason.

As some relief from that channel problem I drew this Tee-nut, and yes its proportions are rather unusual because it is for a real purpose: to fit a boring-table for my Harrison lathe. That was made by its former owner, and he must have used those slot sizes for a reason. I bought it via a sales advertisement on this forum.

Apart from wanting a set for its future use anyway, I am considering whether to machine it out to accommodate the compound slide as on the standard cross-slide, so giving an equivalent to the smaller Myford arrangement. So by suitable Tee-nuts first I can clamp it to the faceplate, it having no through-holes.

The weather is slightly warmer today so I spent a happy hour or so in the workshop this morning, measuring and experimenting with tool-holders etc. It is higher than the normal cross-slide so I’ve to consider tool choice and setting.

 

As far as using Alibre goes it was really an exercise in making these constraints work, though its sketches were never fully-defined. On the first go I’d made the upstand too narrow (typing error), and I took several attempts to realise it would work by producing the replacement sketch on the central plane, not end face. Unless I could have used the face with a different extrusion choice.

 

 

[JasonBModerator @jasonb]

You are picking it up. Good to see you have it centred up and have extruded mid plane which then makes placing the hole easy as it will snap to the axis.

 

when you get a moment have a go at altering your chassis file, you now have the altered ones I sent that you can also look at for reference.

Do you fancy having a go at a rough representation of the boiler and getting that assembled between the chassis next?

[Nigel Graham 2Participant @nigelgraham2]

I still can’t get it.

I’ll just have to accept I can’t use the Sweep tool.

After several attempts I appear to have the two figures on the right planes, I think, with the section even facing the right way, but that’s far as I can go. I still don’t really know what I did, though.

I’m not helped by the error messages being ones only the experts would understand, but the experts never do anything to make such things appear anyway:

[David JuppParticipant @davidjupp51506]

Nigel,  please send me the file that contains the error – I’ll work out what went wrong and let you know.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou David.

Well, I tried to.

Only I found I’d closed it un-saved I have only the earlier failure, but I can’t re-create the above version because it took several attempts in different bits of it, and I don’t know what I did.

I think what’s happening is that the Sweep tool has gone beyond difficult and become impossible for me. That phenomenon is not confined to my attempts at CAD. I’ve had similar stops in other, very different areas; I cannot help them, have no control over them, and they are permanent.

 

One my fellow club members once admitted failing completely in trying to learn CAD – I don’t know what make. I don’t know what his profession was either, but it was obviously high-grade, high-paid, so he was obviously much more intelligent and educated than me, probably with a Degree or higher. If someone like him can’t learn the subject I’ve no hope.

[David Jupp]

On David Jupp Said:

Nigel,  please send me the file that contains the error – I’ll work out what went wrong and let you know.

Please permit me to say … this is an astonishing level of support, and if Alibre Atom was a available in a MacOS version, I feel sure I would be using it by now.

MichaelG.

[Nigel Graham 2Participant @nigelgraham2]

It is, Michael, and I am very grateful for it.

Sadly, I couldn’t send the file. I found I’d not saved that last edition illustrated above, as I explained above.

[David JuppParticipant @davidjupp51506]

Well the error message didn’t obviously coincide with the most common errors people make with sweep, though I can’t rule those out.

I also note that there was, or had been, at least one more sketch in the file.  I can’t be sure the correct sketches have been selected for the sweep.

The most common problems seen with sweep are;

• The path includes a radius too small for the profile to be traversed along the path – think like a hose that is kinked.
• The path doesn’t reach the plane that the profile sketch is on.
• The user has mistakenly specified the path sketch as the profile and vice versa.
• The path sketch includes overlapping or intersecting figures.

I can’t rule out other issues, in the file.

I’ve asked repeatedly that Nigel saves files when he hits problems, and sends them to me for analysis.  So far Nigel hasn’t done that.  Without evidence from the files, there’s a limit to how helpful I can be.

Error messages often originate from the ACIS modelling kernel, and yes those can be cryptic, often because they describe a generic issue in mathematical/geometric terms rather than relating to the specific case that the user is attempting.

[lekmirParticipant @lekmir]

I’m shaking my head in disbelief, so I spent 5 minutes with my beloved Onshape and created something resembling Graham’s channel. Then another couple of minutes to obtain the “workshop drawing” so desperately needed by Nigel, and adorned it with some dimensions.

But no one can be forced to his luck (not sure if that saying is used in England)

Regards,
Hans

 

…

[Nigel Graham 2Participant @nigelgraham2]

Edited because a bit of cross-posting went on there.

I didn’t delete the file deliberately, but simply forgot when I closed it.

.

Meanwhile I tried once again creating the chassis rail from the three Part files of separate sections of modelled channel, but that Assembly is even harder than this Sweep method I can’t understand.

I experimented with another possible way, but although that failed as well it showed I could represent the frame by just the vertical webs, omitting the flanges. So that’s what I’ve done.

No of course it’s not realistic but it’s obvious by now this is the only way I can model a frame like this in 3D. The internal dimensions are the ones that matter anyway. Most major components are bolted to the flanges but I expect they’ll be happy screwed to thin air. I can show only their very basic outlines or even just envelopes anyway, certainly no details, here. I’d have to add them to this drawing, if it will let me, as if all one “Part”, not as an Assembly from separate drawings.

Ideally the XY plane should be on top of the webs, not their undersides, because most of the rest of the components are on top of the channels.

There are two other cross-members to fit in there, on that tapering section, but I need verify my measurements.

[JasonBModerator @jasonb]

You should only need the lengthways position of that cross member.

Select one of those extra central planes you have added, sketch the cross section of the crossmember not the top. and then extrude “to geometry”. This will give you half of it which can then be mirrored about the same plane.

[Nigel Graham 2Participant @nigelgraham2]

Thank you Jason.

Also, thankyou David for sending what the rail should look like.

Ironically I realised only this morning when thinking about what I need re-measure, that for practical purposes I need only that trapezoidal centre section.

It will hold the engine and transmission, which have to be connected around the final-drive chain sprocket whose location became fixed by the axle and radius-rods I made too many years ago.

If I ignore everything outside that tapered area, I might be able to draw just that part of the frame correctly. They consist of the two side pieces and one cross-member, all channels; and a second cross-piece, of angle-section. Still problematical though, because the outline is a trapezium, not a rectangle.

 

If modelling the entire chassis I could represent the channel members as solid bars – but why even try to model the full chassis?

There is no point trying to model the whole vehicle in 3D CAD, even heavily simplified. If I tried it, it would be very incomplete as I’d have to simplify much of it and omit everything too hard to draw, including the steering links, springs, brake rigging, boiler fittings and pipework. This beast is proving easier to build than to draw, despite continually having to revise existing parts and overcome built-in errors!

I don’t know why I thought I would eventually be able to model it in 3D CAD. I think someone here suggested it. Aye – them as finds very hard things easy, tend to think those easy for everyone.

.

I need draw the machinery properly, but almost everything forward and aft of that machinery space is nearly complete, made mostly without drawings, though needing a lot of finishing and some revising.

There are “only” two major items to make other than the engine and road-gearing:

– The proper steering gear-box to replace the present, temporary arrangement. That needs proper drawings. I might be able to model its components in Alibre, with suitable simplifying; but not the assembled mechanism.

– The boiler cladding sheets. They cannot be drawn using CAD, only marked out from cardboard templates measured and cut to fit  (The other “CAD” !)

[Nigel Graham 2]

On Nigel Graham 2 Said:

 

– The boiler cladding sheets. They cannot be drawn using CAD, only marked out from cardboard templates measured and cut to fit  (The other “CAD” !)

Well they can – but admittedly not in Atom3D.  Alibre Design Expert does have a module for Sheet Metal parts.  It can unfold the 3D design into a flat pattern for cutting, and calculates the bend allowance whilst doing so.

[Nigel Graham 2Participant @nigelgraham2]

If I struggle with Atom, Alibre’s full editions would be too ambitious!

The sheets need wrap around two intersecting cylinders, and I recall enough A-Level Technical Drawing to be able to determine a method for this problem, though based on measuring the physical thing.

Developments are also covered in old text-books I have, but at least in this case I would not need consider bending allowances I recall having to apply as best I could to thicker metal, from the table in the ‘Zeus’ Book. The really difficult part would be a joint cover for the interpenetration itself.

[David JuppParticipant @davidjupp51506]

Nigel – I was not suggesting you try it.  I was only responding to your assertion that they cannot be drawn in CAD.

A cover for the interpenetration might be beyond Alibre’s Sheet Metal capability as it involves stretching/shrinking the metal in more than one direction.

[JasonBModerator @jasonb]

One can still use the CAD model to developed the true shape just like you did back at school. Easy to divide the circle into 12, add a few construction lines and take measurements off to plot and then use a spline to join them. Circumference can be taken from the 3D model and the part “stretched” in the required direction to give the bending allowance.

OK it is not as easy as a full sheet metal program but the CAD can still help a lot

I’ve certainly used my CAD model to produce DXF files for laser cutting of parts that were subsequently bent to follow a curve and or taper in one or two directions and they worked out fine.

[Nigel Graham 2Participant @nigelgraham2]

David –

I know but the last thing I want at the moment is what the most advanced CAD tools can do. That only stresses how little progress I can make.

 

Jason –

There isn’t a “bending allowance” to worry about here, just a small overlap along the length.

The awkward bit is the joint cover, which will have to be shaped over a former. It is probably not essential functionally but it would hide what would otherwise be very unsightly.

Anyway… I think some two hours later, nearly a dozen sketches and dozens of Faulty Sketch error-messages that don’t indicate which Degenerate Open Loops are Overlapping which Intersections, I finally modelled the frame’s central section as a single part to resemble something like intended. The rearward cross-member is right: it is angle, not channel.

I’d have needed fewer extrusions if I’d not forgotten the outside flanges until after I’d mirrored the first nearly-half. I did though speed up production by plotting and extruding the upper ones “accurately” then turning the thing over and simply tracing their images to make the lower ones. It didn’t occur to me until typing this I could have mirrored them but as I’d have needed create an equatorial plane for them, it would not have been much less work.

Still, though it’s rough it does at least resemble the real metalwork and is to size in the right places. Hopefully. Is it possible to add the webs and flanges then a little fillet to give a more life-like appearance?

[JasonBModerator @jasonb]

Looks like you have the webs and flanges so not sure what you want to add there.

Fillets are quite easy. make sure you have saved what you have got then along the top you have the “fillet” tool so click that. It comes up with the default fillet radius highlighted which you will probably need to change from 0.5″

Then click in the larger box “entities to fillet” so that gets highlighted

You can now click any internal corner on the 3D part and that should immediately show a yellow fillet, keep clicking the ones you want then say OK. Sometimes if there are a lot it is worth doing a few batches rather than all at once.

The same procedure if you want to round over an external corner eg if you channel is bent from flat.

Be careful not to click a face as that will both round any external edges and fillet any internal. If you do locate it in the entities box and delete just that item

You should not have too many problems with what you have there, sometimes filleting odd junctions like a cylinder meeting an ellipse can throw a bit of a wobbly.

 

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