Making a Start in FreeCAD

[SillyOldDufferModerator @sillyoldduffer]

Part 1

As getting started with 3D-CAD is a problem I recently outlined how to get FreeCAD into a position where a beginner could start modelling. FreeCAD is of interest because it’s Open-Source free, not because it’s the best possible CAD choice. I find it handy for simple work, and as a safety-net in the event Fusion360 becomes unaffordium. The ‘starter’ piece got some positive feedback and a PM conversation about finding up-to-date FreeCAD Tutorials with Thor inspired me to show what happens once FreeCAD is ready to go. The idea is to get people started by demonstrating how straightforward it can be to 3D model simple objects without plunging into shark-infested depths. I’m not competing with the Alibre thread!

Here’s the example. It’s the key used on my lathe’s 4-way tool-post.

For objects this simple, I’d do a ‘back of an envelope’ sketch. A rough drawing capturing the shape and dimensions needed to make the item is good enough. It’s a memory aid rather than a technical drawing. However, sketches like these are a good way to prepare for a 3D CAD model.

For more complicated objects or drawings other people will work from, I do ‘proper’ technical drawings. These can be done by hand on a drawing board, but I prefer a computer. I use QCAD. With practice it’s faster than rule and pencil, and far neater, especially after multiple mistakes are corrected with a grubby rubber!

Behind the scenes 2D can be messy! Here's with construction lines:

Proper technical drawings are skilled work. As an amateur I claim the example above to be a ‘First Angle’ Drawing, but I might be wrong! Also, trained draughtsmen may not be impressed by my treatment of dimensions, line thickness or labelling. Nonetheless, I believe it’s clear enough to be used by someone else to make a tool-post key.

Two major problems with 2-Dimensional technical drawings. First it’s necessary for the draughtsman to mentally translate a 3D object correctly and unambiguously into groups of 2D views. Secondly it’s necessary for the user to translate the group back into a 3D object. It helps if both understand and follow the same conventions and neither blunders during translation. Mixing up the difference between First Angle and Third Angle can be desperate because the made object could be a mirror image of that intended. Most modern drawings are Third Angle, older European drawings are usually First Angle, and amateur drawings can mix both in the same plan or be neither. Much opportunity for confusion.

Questions and comments welcome.

Dave

[SillyOldDufferModerator @sillyoldduffer]

[SillyOldDufferModerator @sillyoldduffer]

Part 2

3D CAD eliminates many 2D drawing errors, and, once mastered, the process is generally quicker. It works by developing solid models, not views. Although ‘Sketching’ is part of the process, it might help beginners to dump the idea that 3D CAD is drawing at all. Think ‘modelling’ instead of drawing, albeit the solid model only exists inside a computer. Seeing the model on-screen in 3D makes it much easier to spot mistakes.

3D CAD offers various ways of converting the model into a real object. For a manual workshop, the 3D model can be rendered as 2D drawings in First or Third Angle. Another output is photo-realistic views of the object, in metal, with or without paint. Yet another representation is a mesh for stress/strain analysis. Another common output is the G-code instructions needed to create the real object with a 3D printer, usually plastic but concrete and metal are also possible. Or the G-code needed to make the object by cutting in a lathe or milling machine. Stamping, grinding, engraving, laser cutting, etching and other manufacturing processes might be available too.

Many human errors are eliminated because the outputs are produced automatically direct from the solid model. In the event the model is changed, it often unnecessary to rework the outputs; asking a computer to generate a complete set of new 2D drawings is much easier than asking Mr Grumpy to start again!

Sadly, these advantages aren’t handed to the user on a plate. The software looks and can be intimidating. As always, best to start simple and work up. Like riding a bicycle, with luck CAD will suddenly make sense.

Here’s the plan:

1. Create the 42mm x dia 12mm centre shank

2. Add the 15mm x dia 18mm top

3. Add the 12mm x dia 18mm base

4. Cut a 8.1mm square hole in the base

5. Add the handle

6. Beautify with Chamfers

7. Generate 2D Drawings.

Start FreeCAD, and follow the earlier instructions to get into the Sketch Editor in the Part Design Workbench. Note that Sketcher Buttons marked with red-dots and white lines are drawing tools, (lines, rectangles & circles etc), while those all in red force constraints, parallel, vertical, distance, diameter, angles tangents etc. Hovering over the buttons should display what they are. Useful tips:

• the ESC key ends the current action.

• On the left-side of the FreeCAD window is a ‘Combo View’ Panel. The ‘Model’ tab lists the steps taken to create the model. It can be used to select and edit previous steps, to hide and reveal them, and to alter the stage’s appearance, including transparency. The ‘Tasks’ tab lists the tools that can be used at the moment. Using FreeCAD involves switching between these two lists.

Using the Circle Radius Tool (which also draws diameters) draw a circle centred near the red dot in the middle of the grid. Don’t worry about the exact size and position; they are ‘constrained’ next.

Constrain the circle to the centre of the grid by clicking the mouse on the two red dots to select them. Once they are both Green click the button marked with the ‘Create a coincident constraint’ button ( Identified by a small red dot ). The circle should jump into position. It is locked in position.

Select the circle by clicking on its perimeter. Then click the red ‘Constrain an Arc or Circle Button’ and set the radius to 6mm. Note the circle goes green. This indicates it is ‘Fully constrained’: it’s a circle of fixed diameter locked in position inside 3D space. It’s not floating about. By no means essential for sketches to be ‘Fully Constrained’ but I’ve found keeping things tight minimises trouble later. FreeCAD, like other 3D software can behave very oddly if a user’s model becomes internally inconsistent. Although this can be very difficult at first practice makes perfect – after a while, modelling becomes second nature. It’s important to obey the software package’s rules, it will absolutely not understand what you meant, only exactly what you told it to do.

Dave

[SillyOldDufferModerator @sillyoldduffer]

Part 3

Now we shall create the middle part of the solid shank by ‘Padding’ the circle. Other CAD packages call this operation ‘Extrude’. Close the sketch editor. In the Tasks Tab in the Combo View should be listed the most common operations likely to be needed next. Keep an eye on the Workbench; much confusion if this quietly changes to one of the others and you don't notice!

Select ‘Pad’ and type 42mm into the Length box before clicking the ‘OK’ button.

A cylinder should appear on screen. It can be rotated using the alignment controls. (Mouse controls also available.)

Next lets add the bottom of the shank. Click on the face at one end the cylinder. It should turn pale green.

In the Tasks List, click on ‘Create Sketch’. This allows us to draw a sketch on the cylinder’s end-face, that can be ‘Padded’ or ‘Pocketed’ to cut a hole. Draw a circle centred on the face and constrain it’s diameter to 18mm.

Close the Sketch Task and, as before select the Pad tool. This time dimension the pad to be Length 15mm, producing an new object that, rotated, looks like this:

Rotate the object and select the other end. Sketch another 18mm diameter circle on it and Pad to Length 12mm to add the base.

Dave

[SillyOldDufferModerator @sillyoldduffer]

Part 4

Now select the new base, and sketch an 8.1mm square on it. Use the ‘Create a Regular Polygon’ tool rather than ‘Create a Rectangle’ . The first positions on centres, the second is on corners. The ‘‘Create a Regular Polygon’ button has a down arrow on the left; clicking it offers a list of possibilities including squares.

Zooming in (try rolling the centre wheel on your mouse), shows the square drawn with several preset constraints. All that’s needed to fully define its size is to select one side and add length 8.1mm with the red I-bar button. The square should also be centred on the base with the ‘Create a Coincident Constraint’ button.

Close the sketch and, in the Tasks pane click the ‘Pocket’ tool. Pocket is the opposite of Pad; it cuts a sketched shape into the solid. Setting length to 12mm creates a square sided socket inside the tool-key’s base.

Brief digression, the similar ‘Hole’ tool specialises in round holes that can be threaded and countersunk etc.

At this stage the shank is almost complete, the main omission being the Tommy bar handle. This introduces a new trick. The obvious way to make the Tommy bar (or hole to take one), would be to sketch a circle on the side of the shank and ‘Pocket’ it. Not quite that simple because CAD tools do not (usually) allow sketches to be drawn on curved surfaces – the geometry is difficult! Instead, the package can add new planes to the model, and these can sketched on to do the necessary. The technique is powerful because planes can be rotated to any 3 dimensional angle.

Select the top of the shank by clicking on it. Then, in the Tasks pane, select the ‘Create a Datum Plane Tool’

With luck the new plane will be oriented correctly. Not so in this example.

Scrolling down the Tasks pane whilst the Datum Plane tool is active reveals that the plane can be offset, and turned (Roll, Pitch and Yaw.) Note the booby trap in the X,Y, and Z offsets, which are set in metres! Fortunately numbers can be typed with a unit, eg. 10mm

All we need to do is turn the plane through 90 degrees to align with the shank’s centre axis. Type 90 into the Pitch Box:

Click the ‘OK’ button to close the Datum Plane Tool. Then select the plane by clicking on it.

Now select ‘Create Sketch’ from the Tasks pane:

Dave

[SillyOldDufferModerator @sillyoldduffer]

Part 5

There’s a problem. Although the necessary circle can sketched on the plane, we can’t see it! The cure is to select the Model tab in the Combo View and Right Click on the bold ‘Pocket’ Line. This produces a list of options from which select ‘Appearance’. Use the dialogue to set Transparency to about 80%, producing a view where the sketch grid can be seen inside the solid shank:

In ‘see through’ mode, it’s easy to draw a circle in the right place on the plane and constrain it as required. Close the sketcher, revealing the result, including internal detail of the square socket.

Press ‘Pad’ but this time also tick the ‘Symmetric to plane’ box as well as Length 100mm

The ‘Symmetric’ option pads sketches in both directions, producing a nearly finished tool-post key. The datum plane (or any other feature listed in the ‘Model’ tab), can be hidden or revealed by selecting it and tapping the Space Bar.

So far, the tool-post key has been modelled by Padding and Pocketing a few sketched circles and a square. Once a solid object has been modelled, there are other tools available. Just as an example, select the lower edge of the key (selection highlights in green), and then click the ‘Chamfer’ tool in the Tasks pane.

Dave

[Rod AshtonParticipant @rodashton53132]

Dave – Excellent thanks. Freecad deserves a UK champion.

Have you tried the CAM as I have not yet?

Rod

[SillyOldDufferModerator @sillyoldduffer]

Part 6

Last step in this introduction is to generate 2D drawings from the finished model. Switch to the ‘Drawing’ Workbench (see pointer):

Click on the ‘Insert New Drawing’ button to make an empty sheet.

Then, select the Chamfer line in the Model list in the Combo View and click the ‘Insert Orthographic Projection of a Part’ button. (The Chamfer line is the last step in the model) Bingo, a 2D drawing should appear.

The Tasks pane has several ‘Secondary Views’ tick boxes. Selecting adds more 2D projections to the drawing, scaling as necessary. It is also possible to show hidden lines.

This is an opportunity to point out that FreeCAD has limitations. Unlike paid for alternatives the 2D generating tool doesn’t support adding dimensions in an integrated way yet. How it can be done is described here.

There are many other examples where FreeCAD either doesn’t support a feature at all, or the way it works is labour intensive! However within limitations, it does a useful job. The way it works is similar to Fusion360, though Fusion is much more advanced.

Dave

[SillyOldDufferModerator @sillyoldduffer]

Part 7

Conscious that I’ve only scratched the surface, I’ll finish with two other quick examples. Say you wanted to model an 18^th century cannon. Pretty clear the way I made the tool-post key isn’t quite suitable. A cannon object can be made thus. Start FreeCAD as describe before but this time sketch half the profile of the cannon. Drawing the lines and arcs etc that outline the cannon requires more sketcher skills than the tool-post key, but the principles are the same. Sketch the lines, constrain them (including making sure their ends join), and then apply a convert to solid tool.

Padding the cannon sketch creates the wrong shape!

Pad is the wrong tool in this case. Using the ‘Revolution’ tool to spin the sketch around the horizontal axis, does what’s needed.

There’s a mistake in the sketch spoiling the cannon model. Zooming in on the cascabel set to 80% transparency reveals a ‘feature’ inside. Mistakes like this can cause considerable bother later on. It’s an unwanted inconsistency, not obvious at first sight, that might confuse when the tool suddenly refuses to perform an apparently legal operation or displays something completely unexpected. As with building a skyscraper you have to take care with the foundations!

The cannon can be bored by sketching a circle on the flat muzzle and applying a Pocket

Last example, the verge, or crown-wheel for a clock:

This is modelled by padding two concentric circles to make a short pipe, adding a datum plane to one side of the cylinder on which the tooth shape is drawn, pocketing the tooth through one side of the cylinder, and then rotate-copying the tooth-shape 13 times around the central axis with the ‘Create a Polar Feature’ tool.

Apologies for the long-winded detail but missing out simple steps in 3D leads to chaos. Once understood, modelling can be rather fast. The models described only take a few minutes to create once you know how FreeCAD works. And far longer to describe!

Dave

[SillyOldDufferModerator @sillyoldduffer]

Whoops first error spotted. The introduction in Part 1 mentions an earlier thread in which starting FreeCAD and getting to Sketcher stage is described. The link to the 'Is CAD For Me' thread is missing.

Dave

[SillyOldDufferModerator @sillyoldduffer]

Posted by Rod Ashton on 19/06/2019 10:26:14:

Dave – Excellent thanks. Freecad deserves a UK champion.

Have you tried the CAM as I have not yet?

Rod

Hi Rod,

Not sure I make any kind of champion! I played briefly with CAM and managed to produce some G-code but still in nappies on that side. Not much incentive to get stuck in alas because I'm a manual workshop. 3D printing is on my ToDo list but it's near the end and it's a very long list!

Dave

[martin perman 1Participant @martinperman1]

Dave thanks for that, will have a play tonight.

Martin P

[Thor 🇳🇴Participant @thor]

Thanks Dave, will be following with interest.

Thor

[Dave Smith 14Participant @davesmith14]

Dave

Well done you have explained the method of simple solid modelling very well (I had about 20/30k hours seat time on CATIA V5 during my working life and still probably do about 500 hours a year in retirement). Although the actual commands will differ the majority of solid modellers from FreeCad, through Fusion 360 to SolidWorks and CATIA all work in essentially the same way. I totally agree with your differentiating between 2D CAD drafting and 3D CAD modelling. It is essential for newcomers to understand what you are creating is a virtual part with, volume, mass etc. 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, in fact at work we taught people who had no engineering experience what so ever how to do quite complex models and to blow down 2D drawings.

Regards

Dave

[Robin GrahamParticipant @robingraham42208]

Thanks from me as well Dave (SOD). No apologies for long-winded detail are needed – for a complete beginner like me that's what's wanted. I've tried, on and off, to get to grips with 2D CAD for years but have always given up in frustration and gone back to pencil and fag packets . I'm actually (so far!) finding the 3D way of working more intuitive.

When following your 'getting started' instructions in the other thread, after drawing the two circles I got a warning that the construction was unconstrained with 6 degrees of freedom. I guess one of those must be that I haven't specified that the circles must be concentric, but I can't see what the other five are. Can you (or anyone else) enlighten me?

Keep up the good work!

Robin.

[Michael GilliganParticipant @michaelgilligan61133]

Posted by Robin Graham on 19/06/2019 22:07:58:

… I got a warning that the construction was unconstrained with 6 degrees of freedom. I guess one of those must be that I haven't specified that the circles must be concentric, but I can't see what the other five are. Can you (or anyone else) enlighten me?

Keep up the good work!

Robin.

.

'6 degrees of freedom' usually means the object is completely unconstrained

… free-to-move in Roll/Pitch/Yaw and X/Y/Z

MichaelG.

[Robin GrahamParticipant @robingraham42208]

Thanks Michael that's helpful – it's given me a better idea of how the program 'thinks'. In particular I hadn't realised that X/Y/Z matters – objects are invariant under translation, it doesn't matter where the thing is my 'screen space'. Until I try to match them up with other things I suppose. So it's like real life! Pennies are beginning to drop.

Robin.

Edited By Robin Graham on 19/06/2019 23:02:41

[Kiwi BlokeParticipant @kiwibloke62605]

Wow! Fantastic! Thank you Dave for taking the time to put such a clear guide together. Over the last year or so, I've installed FreeCad – and removed it in disgust – a number of times, having got nowhere. Today, I followed your guide to the end, with success! But what a tortuous process. I suppose that with practice (how much) and a comprehensive background knowledge of the application, its use becomes second-nature – but, until then…?

Locating the hole for the T-handle took a bit of guesswork. However, a guide such as this should not spoon-feed us with every minute step, should it?

The chamfer tool seems also to add fillets to the selected surface. How do you remove them, or have I done something stupid?

I haven't been able to install freecad-doc: it seems to be incompatible with the latest (Linux) version of the freecad package. This seems to mean that off-line help isn't possible. Again, have I been stupid?

[Thor 🇳🇴Participant @thor]

Hi Kiwi Bloke,

I am trying to understand FreeCAD and have found a few tutorials that you may find helpful:

***Link***

***Link***

***Link***

***Link*** (manual)

Thor

[Thor 🇳🇴Participant @thor]

Following Dave's excellent tutorial I tried to make a model of something useful, a tray for my ER 16 collets. A friend of mine has access to a 3D printer where he works. I haven't tried printing the model as my friend is on summer vaccation.

I have tried to write an explanation of what I did here, probably many errors so I assume I will have to revise it.

Thor

[SillyOldDufferModerator @sillyoldduffer]

Posted by Kiwi Bloke 1 on 20/06/2019 10:55:00:

…

But what a tortuous process. I suppose that with practice (how much) and a comprehensive background knowledge of the application, its use becomes second-nature – but, until then…?

Locating the hole for the T-handle took a bit of guesswork. However, a guide such as this should not spoon-feed us with every minute step, should it?

The chamfer tool seems also to add fillets to the selected surface. How do you remove them, or have I done something stupid?

I haven't been able to install freecad-doc: it seems to be incompatible with the latest (Linux) version of the freecad package. This seems to mean that off-line help isn't possible. Again, have I been stupid?

Tortuous process indeed, and I reckon it's what puts people off. Although the steps are simple enough one by one, it's not immediately obvious what they are, or that they have to be in a logical construction order.

It's not like 2D where lines can often be drawn in any order. 3D-Cad is more like real-world making were things are made by cutiing and joining. As we've all learned painfully, the order operations are done to lumps of metal matters very much! With practice 3D-CAD is rather like actual machining; first time I cut a thread on my lathe it seemed unbelievably complicated, what with change-wheels, angles, tpi, pitch, thread-dials, depth of cut, measuring, metric vs imperial and crashing the saddle. Now I've cut a few dozen threads I'm not sure what the fuss was! Like real world machining, I suspect a common mistake is not practising enough before moving on to complicated objects.

Sorry about the T-bar; I removed a paragraph to clarify the steps and never put it back!

There seems to be a problem with the FreeCAD package; I'm loading the very latest version from the Ubuntu ppa, and attempting to install the local documentation breaks it! Almost certainly a mistake made by the packaging team that will be corrected later. So you're not stupid – me too!

Fillets and Chamfers? Not quite sure what you mean. Do you have chamfers that look like fillets?

In this object, the top is rounded with a fillet, and the other levels are chamfered flat. (The effects are done with different tools, their actions recorded as 'Chamfer', 'Chamfer001', and 'Fillet' in the Model time-line list.)

Do you mean, how do I remove an earlier chamfer?

Dave

[martin perman 1Participant @martinperman1]

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

[VersabossParticipant @versaboss]

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

[SillyOldDufferModerator @sillyoldduffer]

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 ColvinParticipant @roncolvin83430]

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.

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