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Making a Start in FreeCAD

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martin perman20/06/2019 13:04:52
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Gentlemen,

Like others I have tried and failed, many times, to understand 3D/2D drawing programmes and have been loathe to buy expensive software to find I dont understand it, Dave has managed to turn my light on by making it obvious, I think I may have found another manual as well, **LINK**

Martin P

Versaboss20/06/2019 13:40:37
461 forum posts
51 photos

I think SOD's tutorial is really what is badly needed for FreeCad. But I really wonder every time why Onshape is never mentioned here (except by me I think!).

I just did SOD's example in Onshape, and it is so much easier. The only thing I would do differently next time would be the cross bar. I have it visually correct, but the build tree shows an error.

Unfortunately I don't know how to insert screen pictures here (except via long winded procedures), but as it is a public part, anybody using Onshape can see it (under SODexample).

Kind regards,
Hans

SillyOldDuffer20/06/2019 14:33:53
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6681 forum posts
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Posted by Versaboss on 20/06/2019 13:40:37:

... I really wonder every time why Onshape is never mentioned here (except by me I think!).

I just did SOD's example in Onshape, and it is so much easier. ...

Kind regards,
Hans

Hi Hans,

The only reason I've never taken an interest in Onscape is the price. The Standard license is $1500 per year and Professional $2500. But is Onshape like Fusion360, with a free version available for hobbyists and students? (Fusion don't exactly make it clear they have a no-fee license for hobbyists, students and small businesses.)

I'm not attempting to convert anyone to a particular package. FreeCAD suits as way in to 3D-CAD because it's Open Source and avoids license problems and the fear that free access to a commercial product might be taken away later. Playing with FreeCAD might waste time but it won't cost money!

Alibre, Fusion, Onshape and others all have significant merit, not least that FreeCAD isn't as slick, advanced or bug-free as any of paid-for products. I switch to Fusion for complicated modelling, multiple parts and joints.

Dave

Ron Colvin20/06/2019 15:22:18
77 forum posts
6 photos
Posted by SillyOldDuffer on 20/06/2019 14:33:53:
Posted by Versaboss on 20/06/2019 13:40:37:

... I really wonder every time why Onshape is never mentioned here (except by me I think!).

I just did SOD's example in Onshape, and it is so much easier. ...

Kind regards,
Hans

Hi Hans,

The only reason I've never taken an interest in Onscape is the price. The Standard license is $1500 per year and Professional $2500. But is Onshape like Fusion360, with a free version available for hobbyists and students? (Fusion don't exactly make it clear they have a no-fee license for hobbyists, students and small businesses.)

I'm not attempting to convert anyone to a particular package. FreeCAD suits as way in to 3D-CAD because it's Open Source and avoids license problems and the fear that free access to a commercial product might be taken away later. Playing with FreeCAD might waste time but it won't cost money!

Alibre, Fusion, Onshape and others all have significant merit, not least that FreeCAD isn't as slick, advanced or bug-free as any of paid-for products. I switch to Fusion for complicated modelling, multiple parts and joints.

Dave

Onshape is free to hobbyist the biggest restriction being, that the free subscription only allows public data. in other words anyone has access to your work.

FreeCAD has the advantage over Alibre, Fusion and Onshape, in regards that , you do not find yourself waiting for the other shoe to drop, and what has been "free" up until now, you are suddenly charged for.

JasonB20/06/2019 16:42:05
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Posted by Ron Colvin on 20/06/2019 15:22:18:

FreeCAD has the advantage over Alibre, Fusion and Onshape, in regards that , you do not find yourself waiting for the other shoe to drop, and what has been "free" up until now, you are suddenly charged for.

Don't include Alibre in that as they don't do free versions, just a fixed term trial which you will then either need to pay for a suitable version to continue or go elsewhere so no sudden hidden surprises as that is up front from the start..

Versaboss20/06/2019 17:28:33
461 forum posts
51 photos
Posted by Ron Colvin on 20/06/2019 15:22:18:

Onshape is free to hobbyist the biggest restriction being, that the free subscription only allows public data. in other words anyone has access to your work.

Yes, what you said is true, but as I think there are thousands of users, and afaik it is not possible to search the enormous list of public drawings. If you want to be safe(r), just give your work a meaningless name.

I had also a look at some Fusion videos, and there and also in FreeCad the author(s) emphasize the importance of 'constraints'. Onshape also uses constraints, but you use them only if you really need them (e.g. make a line tangent to a circle, or parallel to another line, or 2 circles concentric.

Another point: I think it is really easy on Onshape's site that it is absolutely free for private use.

Regards,
Hans

Edited By Versaboss on 20/06/2019 17:29:23

Kiwi Bloke20/06/2019 22:26:43
500 forum posts
1 photos

It's sometimes difficult to remember individual steps made when blundering around in the semi-dark... I think I selected the surface to receive the chamfer, expecting the chamfer to be applied to its external arris. Lo and behold, a chamfer was produced, but simultaneously also a fillet in the internal 'corner' at the junction of the larger and smaller diameter of the body of the key. Impressive and pretty, but was that what was intended...?

Bazyle20/06/2019 23:04:43
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5698 forum posts
208 photos

I tried Onshape when It first became available but it wouldn't work on MS Explorer so I had to get another browser which my work IT didn't approve of. Then at home I had the problem of it being all online and my internet at the time being super crap that wasn't much fun.
Then we had a demo at EDMES of Fusion with the speaker showing that it could work a fair bit offline so I had a go at that and found it quite good.
I then tried the Alibre offer and thought the permanent ownership would be a plus but in the end I haven't found I actually use any CAD enough (at all apart from the examples) to be worth paying more than about £50 for but it was nice to have the 'lessons' in MEW.
I found Freecad and it seemed to be rather nice in having lots of different modes, drawing, architectural, sketch etc. However I have then been getting confused deciding which of the tools to use.

SOD's intro here is fantastic - The equivalent of the MEW articles so just what I want. Well done that man. I hope some more will follow.

Nigel Graham 220/06/2019 23:06:48
913 forum posts
16 photos

I read the above with interest to see if FreeCAD might just possibly be simpler than TurboCAD.

However I saw that, Dave Smith 14, your remark,

" I particularly hope Nigel Graham2 reads this and has a go following the guide lines you have described. It is not rocket science using 3D modellers,... "

No it isn't - and the designers of Yuri Gagarin's capsule had to make do with their People's Glorious parallel-motion drawing boards, like the one likely to remain in my dining-room for my benefactors.

Unfortunately my experience with TurboCAD and brief excursions into other makes shows 3D modelling is literally too much for me; in quantity as well as difficulty. It's unlikely then I could follow your third-party suggestion.

'

TC differs from Alibre, FreeCAD, Fusion etc. in giving a direct 2D or 3D, choice. I think you can take elevations from its model views, but I don't know how.

I can use TurboCAD enough for rather rough orthographic drawings, manually editing the approximated dimensions so they read the right values on prints to anything but scale.

I don't normally find 2D drawings the perceptual problem others claim justifies CAD 3D pictorial models, unless the elevations are particularly complicated. I am used to many years of reading orthographic engineering drawings and Ordnance Survey maps. However I first encountered at work, the 3D picture on the workshop drawing to help the machinist visualise what the CAD draughtsman thinks feasible to machine. Hemingway Kits do that too - but on designs feasible to machine!

I am aware of the trap of mixing First and Third Angle with the risk of mirror-imaging or similar errors. (Hence the convention of a simple cone with end elevation in the drawing's title block.) I expect CAD holds its own traps for the unwary though.

SillyOldDuffer21/06/2019 13:08:12
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Part 8

Many simple parts can be 3D modelled with only the Pad, Pocket and Revolve tools. For that reason it’s worth practising with them several times. Early on keep it simple, pick simple shapes, and don’t be discouraged when you hit brick-walls. They may be because imagination has failed, more likely another modelling tools is needed. Understanding which CAD tool to use is part of the learning process, akin to knowing when to use drills, 2-flute cutters, 4-flute cutters, or fly-cutters in a milling machine.

As the world is complicated, so are the 3D tools needed to model real-world objects. Faced with a new 3D-CAD package, the sheer number of options available is intimidating. Don’t panic: it might take time to crack the code, but the more you explore the easier it gets. You don’t need to learn everything; chances are hobby metal workers are making relatively straightforward shapes, not designing the sweeping plastic curves added to beautify vacuum cleaners!

This example shape is used for everything from ice-cream containers to wheelie bins. It needs a new tool.

dsc06129.jpg

‘Lofting’ is the CAD process of generating shapes in the gap between two sketches. Be warned, loft is somewhat fiddly in FreeCAD. If something doesn’t work, go back and try again. One cause of bother is that given a few possibilities, the software may not select what the user intended. Sometimes helps to rotate, zoom-in or hide features to make sure the correct object, face or edge is selected.

First open the sketcher and draw a rectangle representing the container’s base. (In the example I’m not bothering to constrain the sketch as would be necessary to model a real container.)

freecadloftbase.jpg

Close the sketch and click the ‘Create a New Datum Plane’ button.

freecadloftdatum.jpg

Now lift the new plane 30mm above the existing sketch by typing 30mm into the Z Attachment Offset. (Watch out! Offsets default to metres. If annoying, before starting a new project have a look at Edit→Preferences→Units. Default setting is MKS: you might well prefer ‘Imperial Decimal’ or ‘Metric Small Parts & CNC’, aka mm)

freecadloftraiseplane.jpg

Close the Datum tool by clicking on the OK button at the top, then click on the new datum plane to select it.

freecadloftplaneselect.jpg

Create a sketch on the new plane. The earlier sketch can be seen underneath. Draw a larger rectangle to represent the top of the container.

freecadloftcontainertop.jpg

Close the sketch, revealing the model now has two sketches.

freecadlofttwosketches.jpg

Click on the ‘Loft a selected profile through other profile sections’ button. Select one of the two sketches. I chose the base.

freecadloft1.jpg

The next dialog requires a ‘Section’ to be added. In this example, it is any of the top four edges of the container. Clicking one edge highlights the loft. (Note a loft can follow more than one sketch at different levels, each defining a section of a complex shape.)

freecadlofttentative.jpg

Clicking the OK button generates the solid.

freecadloftsolid.jpg

More...

SillyOldDuffer21/06/2019 13:08:32
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6681 forum posts
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Part 8B

A solid ingot isn’t quite a container yet! To convert it, first hide the datum plane. This is needed because we have to select the top surface of the ingot for the next operation. Hide the plane by selecting it in Model list and tapping the Space Bar.

freecadloftdatumhide.jpg

With the datum plane hidden, select the upper surface of the ingot

freecadloftselecttop.jpg

Click the ‘Make a thick solid’ tool. (Top right under pointer in next picture.)

freecadloftthickness.jpg

freecadloftfinished.jpg

Whilst an object shaped like an ice-cream container might be made of sheet metal or even milled from solid, more likely the ‘Make a thick solid’ tool is of more interest to the 3D printing fraternity. In FreeCAD, the ‘Path’ workbench is used to generate the necessary G-Code. It comes with buttons for selecting tools, simulating cutting paths, facing, drilling and various other operations. I’ve never used it! The CAM process begins with this ‘Job Edit’ dialogue.

freecadpathwb.jpg

Dave

Kiwi Bloke23/06/2019 12:41:01
500 forum posts
1 photos

It's great to see a champion of Free software, isn't it? Is part of the enthusiasm for other packages expressed by others a reflection of the amount of money they have forked out? However, I digress...

I've pm'd SOD about this, but don't want him to feel he has to waste time finding the answer. Far better that his excellent tutorial continues.

Here's the problem. When I applied a chamfer to the annular surface at either of the junctions of the two different diameters of the shank of the chuck key model, FreeCAD produced the expected 'external' chamfer, but also an internal 'fillet' (as would be produced by a V-shaped turning tool). I haven't found a way to restrict chamfers (or what FreeCAD calls 'fillets', but what I call 'corner-rounding' to external edges only. Anyone any ideas - without getting deep into python?

Thor23/06/2019 14:04:40
1324 forum posts
40 photos
Posted by Kiwi Bloke 1 on 23/06/2019 12:41:01:

Here's the problem. When I applied a chamfer to the annular surface at either of the junctions of the two different diameters of the shank of the chuck key model, FreeCAD produced the expected 'external' chamfer, but also an internal 'fillet' (as would be produced by a V-shaped turning tool). I haven't found a way to restrict chamfers (or what FreeCAD calls 'fillets', but what I call 'corner-rounding' to external edges only. Anyone any ideas - without getting deep into python?

That is a bit strange, I just tried to make an external chamfer, and got no fillet (I also chamfered the free end):

toolkey01.jpg

On the other end I tried to just make the fillet, and got no chamfer:

toolkey02.jpg

I don't know what happened, are you sure you clicked on the circle line, not a surface. If I click on the ringshaped surface and chamfer I also get a fillet.

Thor

 

 

Edited By Thor on 23/06/2019 14:05:03

Kiwi Bloke24/06/2019 00:07:57
500 forum posts
1 photos

I thought I'd replied, but my post seems to have got lost.

Problem solved!

Thanks Thor, you've got it! Clearly FreeCAD is smarter than this operator. I hadn't realised that the chamfer tool produces different results, exactly as you describe, depending on whether a surface or edge (line) is selected. I had indeed selected a surface to be chamfered, so FreeCAD obligingly found every edge and did its thing.

Apologies for stupid, unintended emojis in previous post. This forum's software has its own ideas about things...

Edited By Kiwi Bloke 1 on 24/06/2019 00:10:47

clogs24/06/2019 07:07:31
587 forum posts
12 photos

me.... just a hopless old guy that would like to learn........

all I want to do is to lay out a new bungalow and a 200m2 workshop......

was told Sketchup was one way to go but they want you to sign up and I guess hopefully forget to cancel after a month.....

I dont need the dog danglee's just something reasonably simple to learn n use...but FREE...

I'll pay where needed but this I guess will be the last use of such a program there's more important stuff to do in the shed.....

thanks

JasonB24/06/2019 07:27:14
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Any of the CAD pacjkages will work for basic floor plans, why not try this Freecad one. You just draw out the walls and can then raise them 1mm or 2440mm it makes no difference.

Bazyle24/06/2019 09:15:37
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5698 forum posts
208 photos

A floor plan is easiest in Word. I did try freecad and some others for that but far too much detail. In Word just use the top and side rulers and draw lines at a scale of half inch to the foot. Easy to draw a rectangle that is the lathe footprint, colour it, rotate and move it around. I have a few 2ft circles that represent the minimum body - me - that I can drag around the workshop to check clearance.

pgk pgk24/06/2019 10:53:11
2024 forum posts
290 photos
Posted by clogs on 24/06/2019 07:07:31:

me.... just a hopless old guy that would like to learn........

all I want to do is to lay out a new bungalow and a 200m2 workshop......

was told Sketchup was one way to go but they want you to sign up and I guess hopefully forget to cancel after a month.....

I dont need the dog danglee's just something reasonably simple to learn n use...but FREE...

I'll pay where needed but this I guess will be the last use of such a program there's more important stuff to do in the shed.....

thanks

I did that very thing 2 years ago when redesigning/extending a bungalow. I bought a cheap (£12) previous edition of turbocad 2d/3d cos I'd used turbocad in the past when designing my clinic. Frankly the limited architectural bits in the general cheap package weren't worth using but for simple plans it's easy enough as probably most packages are. I still roughed it out on scrap paper first but once the plans are drawn on screen it's easier to rub-out and move stuff.
200m^2 shed... depends what you plan on dragging in there.. but 2M wide by 100M long and all the machines on one side leaves you with a nice shooting range for archery if the roof is high enough

pgk

Thor24/06/2019 14:23:21
1324 forum posts
40 photos

I kind of managed to model Dave's cannon:

cannon.jpg

I left Transparency at approximately 30% to reveal some of the internals.

Thor

SillyOldDuffer24/06/2019 15:26:07
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6681 forum posts
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Posted by Thor on 24/06/2019 14:23:21:

I kind of managed to model Dave's cannon:

cannon.jpg

I left Transparency at approximately 30% to reveal some of the internals.

Thor

Very good Thor, much better than mine. Here's something to try. Because the cannon is modelled as a solid, FreeCAD knows where the Centre of Gravity is. In a real cannon the trunnions should be positioned a little forward of the centre of mass such that the gun is balanced slightly base heavy. Makes it easier to adjust elevation with a wedge or screw.

Here's how to find out in FreeCAD by adding a local coordinate system.

freecadnewcoord.jpg

Select the whole cannon then click on the 'Create a new local coordinate system' button (under mouse pointer above). Then choose 'Inertial CS' as the attachment mode. In my example the Red X and Green Y lines can be seen marking the balance point.

Try it on your cannon to see how well your trunnions are placed! Quite often if it looks right it is right.

Dave

Edited By SillyOldDuffer on 24/06/2019 15:29:20

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