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-   -   [TUTORIAL] 2D Design With Solid Edge (http://forums.overclockers.com.au/showthread.php?t=960755)

Bastard Child 22nd May 2011 1:35 PM

[TUTORIAL] 2D Design With Solid Edge
And the Lord said: "Let us rock" :thumbup:

Quick Navigation: Modelling Tools Dimensioning Advanced Sketching Variable Tables Drafting Tools Sheet Metal

Solid Edge 2D by Siemens PLC is a free 2D drafting package available for download here (420MB or 6hr download @ 20kb/s). To install it I had to turn off Windows UAC and reboot first (instructions here), other than that it's a pretty standard procedure - remember to restore UAC and reboot again.

Once installed run the shortcut and 'start a new drawing':

For a rough tutorial based on an old version of Edge: PDF warning
Here's what I'll typically use for A4 drawings - hosted by OCAU here (right-click, save link as)

The first thing you'll want to do is turn ON the 2D Model Sheet because modelling parts on a 'drawing sheet' is just fucking foolish (we'll cover drawing sheets later):

Some of you may want to turn on autosave, redefine zoom settings, change the colour scheme, increase undo steps, etc:

Note that we haven't set paper size or scale, etc. All design work is carried out at 1:1 on model space and we set those things up later when we switch to drafting.

Some people choose to use a drawing grid, but I find it unnecessary and it tends to clutter the page:

Relationships: Unlike drafting packages of old where you just threw lines around the page and dimensioned them later, good modern software is designed around parametric/relationship design - this means each line you draw will be somehow related to other lines on your page.
-Lines can be snapped together at their endpoints, midpoints, tangent to arcs, perpendicular to another line, offset at a specified distance, mirrored, etc.
-Relationships are permanent until broken or deleted, and we should aim to fully constrain every line on the page.

Example: We have two lines on a page. The top drawing is the old way of doing stuff - you draw simple lines and they can move independantly of each other. The bottom sketch has a 'connect' snap joining the lines, and this relationship is maintained as we drag the lines around the page:

To enable relationships (fuck knows why it isn't on by default) refer to the red bit here:

With relationships ON I can draw a box of any size and the thing will be squarish with vertical sides and a flat bottom, and all the corners to be joined together:

By the way - Intellisketch is a dynamic mouse cursor that shows you how your line will be placed on the page in relation to other lines and important references. Here the line I'm drawing down will be both vertical and on the same horizontal axis as another line's end point:

Fully defining a sketch by using relationships and dimensions is critical because at some point you're going to go back to modify a sketch, and you don't want it all turning to crap!

How to check your design to see if it's fully constrained: Click Relationship Assistant -> Drag a selection box around your model -> click Show Variability multiple times to see what lines are not restrained (also refer to number box):

Example: Here's a quick sketch of a random shape. Everything looks ok at this point, but let's say we want this shape to be taller by modifying the 44mm dimension:
http://i20.photobucket.com/albums/b2...h_70d79efa.jpg http://i20.photobucket.com/albums/b2...h_69b6068b.jpg

Oh dear... we moved the right hand side, but the left hand side didn't move with it. Let's check to see what line(s) still need to be constrained:

You have several options, depending on how you want this line to behave. The obvious solution is to put in a dimension to fix the height of the line from a set point, OR, you can force the line to be in a co-linear relationship with the line that is already dimensioned!

But which method is correct?

Design Intent: Another important aspect to design is capturing your intention. How do you want the model to behave if dimensions are changed?

Have a look at the following two plates and what happens to the hole after length and width are changed:

The left hand design kept the hole at the same the physical distance according to the dimensional constraints we used, whilst the right hand plate kept the hole centred according to geometric constraints (hole was placed on the midpoint of a line that itself was placed on the mid-length of the plate).

So which design is correct? Well that depends on what the designer's intention was...

Layers: Last topic before you bastidges can be let loose drawing. Layers are important because it's how you turn off lines and dimensions without having to permanently delete them - a quick example is the use of construction lines that you don't want printed or visible, but are handy to keep for future use.

Find layer crap here:
http://i20.photobucket.com/albums/b2...h_1885ae45.jpg - those layers circled are ones I commonly use

Bastard Child 22nd May 2011 1:35 PM


For a rough tutorial based on an old version of Edge: PDF warning
Here's what I'll typically use for A4 drawings - hosted by OCAU here (right-click, save as)

Sketching (modelling) is where we'll throw lines down onto the 2D model page, across multiple layers, and fully constrain the sketch so that all lines behave by rules we set. Remember - any dumb fuck with opposable thumbs can draw and call themselves a designer, so let's be a little bit professional about this eh?

Don't be afraid to experiment. If something fucks up just hit undo, or close the file and start the sketch from scratch.

There's two basic approaches to drawing - either draw line segments to the correct length as you go, or draw the basic shape of the object and go back and put in correct lengths. I use a bit of both methods...

Ok so let's draw the following shape - we'll draw it a few times, and I'll add sizes and such later:

Design Intent - look closer at the drawing.... see how it forms a cross shape that's sort of symmetrical, note that lines are vertical and horizontal and meet at 90o, that arcs roll neatly to meet straight lines forming smooth transitions, the slot nestles neatly inside the outer arc of the cross, etc.

You didn't draw it... you don't know what it's used for... you probably don't have the technical vocabulary to describe what you're seeing... but, if I give you this picture:

...I'm betting you'll easily spot it's not designed with the same intent as the first shape:

Congratulations you're now slightly less of a dumbarse than when you got up this morning!

Pencils Ready: From previous topics, your starting point should be:
-2D model space
-Layers set up correctly
-Relationships enabled
-Intellisketch enabled
-Home ribbon visible
...And before any drawing is to be done, set your 'origin' by drawing an X-Y axis (I draw a vertical and horizontal line, 100mm long):

Drawing Origin: To make an origin, go to the construction layer (double click and make sure the pencil icon is there):

Select the line tool, set the type of line (I use center), colour, etc:

To draw a basic line, there's a few options:
http://i20.photobucket.com/albums/b2...h_d6ac3954.jpg (1) We can specify a length and angle first and left-click to place it on the page in one go
http://i20.photobucket.com/albums/b2...h_88990afe.jpg (2) Or we can left-click the page for a start point and then enter data to place the end point
http://i20.photobucket.com/albums/b2...h_25b575a6.jpg (3) Or we can click twice on the page for start and end points, and then edit the line's properties

So we have our first line down and now we can start another line by snapping to any end point of line 1 (note the 'end of line' snap icon):
http://i20.photobucket.com/albums/b2...h_5c75a18e.jpg Take note of the icons used for relationships. Here we have couple of "+" symbols indicating a vertical or horizontal line, and a 'box with a dot' indicating a joined line

Finally, click the lock icon and lock these lines so no further changes can be made to them (this is why I don't bother with grids, I make my own starting point):
http://i20.photobucket.com/albums/b2...h_ad9247cc.jpg Note the lock icon

Feel free to move to the 'outline' layer to begin drawing stuff:

You can hide any layer that you're not currently drawing on:
http://i20.photobucket.com/albums/b2...h_087e87b4.jpg We'll leave the construction layer (drawing origin) OFF, for now...

Sketching: As mentioned at the start of this topic we can either draw an object to the correct size, or roughly draw the right shape and add sizes later. I'm going with the second method because you need to appreciate how important relationships are without being distracted by dimensioning.

So, let's make a copy of this:

-Work on the Outline layer
-Relationships ON
-Intellisketch ON
-Visible line type (just a generic, black, continuous line)

Click the line tool and draw straight lines, making sure they meet at end points:

You can always go back later and add any relationships you've missed. Here I've clicked the Connect tool, then picked the two ends to join:

Followed by the Horizontal/Vertical tool to move the the line segment. Click the tool, then click each end of the line to move it (Solid Edge will move the line to the closest orientation):

Sometimes the line will orientate vertically when you wanted horizontal. Click undo and move the line closer to the final position you desire, and try again.

Next add arcs to the ends - Tangent Arcs are semi-intelligent in that you place the first point down then drag the cursor in the direction and shape you want:
http://i20.photobucket.com/albums/b2...h_798fda00.jpg Have a play, see how it behaves

Second click to place the arc down:
http://i20.photobucket.com/albums/b2...h_2288bd20.jpg Note the symbols for tangent, end point connect

The other arc has gone a bit ferral:

Which is easily fixed by manually adding a Tangent relationship (click tool -> click each line segment you want to apply it to):

Slots: Solid Edge, unlike other apps, doesn't have a dedicated tool to draw slots. Two common methods shown below:

Method 1 is done with 2 circles -> joined by lines -> excess trimmed:
http://i20.photobucket.com/albums/b2...h_603ae27a.jpg http://i20.photobucket.com/albums/b2...h_b6275169.jpg http://i20.photobucket.com/albums/b2...h_792d20c4.jpg

Method 2 is done with 2 straight lines, then joined by tangent arcs:
http://i20.photobucket.com/albums/b2...h_1aaf2bae.jpg http://i20.photobucket.com/albums/b2...h_7ef86354.jpg

I've purposefully drawn stuff at odd angles so you can see how to fix it... here I've applied horizontal relations (which is all the first slot needed), and I'm about to add a couple of missing tangents:
http://i20.photobucket.com/albums/b2...h_76cc2c81.jpg http://i20.photobucket.com/albums/b2...h_e79d89c2.jpg

Don't need two slots, so drag a selection box around one and delete:

Here I've made the slot smaller by clicking on lines and dragging the shape around via end points:

Dragging a selection box around the shape lets you move it into rough position:

We now have the basic shape, and with plenty of dimensions we can constrain the thing from moving around.

The end.

Again, any monkey can throw lines around a page. Let's get some bondage action relationship constraints going.

Co-linear: Straight lines on a page that lie along the same axis can be put into a collinear relation:
http://i20.photobucket.com/albums/b2...h_09722272.jpg do the same with the other pairs of lines...

Concentric: Arcs and circles that nestle within each other have a concentric relation:
http://i20.photobucket.com/albums/b2...h_3fc36993.jpg http://i20.photobucket.com/albums/b2...h_17e5ad5a.jpg <- note that slot size still changeable

Equal: Lines that are the same length can be linked together with the equal tool. Go back and study the original image:

Let's assume that each arm of the cross is going to be the same thickness:

For the Equal tool to work, it needs a line segment to act on. Here I've gone back to the Construction layer and added a line across the arc:

Could have drawn the vertical line in a few other locations:


Note that due to existing collinear relations, we only have to link those 2 lines and not each of the 4 ends of the cross:

Have a think about why I chose to draw the vertical line on the construction layer...

Fillet Curves: It's at this point I've remembered we need a couple of fillets added to the sketch. Fillets have a habit of breaking relations so pay attention to your drawing as you place them. Here I'm adding a couple of fillets, then making them Equal radius with the relations tool:
http://i20.photobucket.com/albums/b2...h_bed8a425.jpg Look - it killed the horizontal constraint. You bastard!

Here I've applied the Equal tool to the fillets and re-applied the Horizontal/Vertical tool to that missing relation:

Let's assume the 4 arms of the cross are the same length... there's a few ways to set the model up to behave this way, but I'm going to draw 2 lines in a cross shape and (1) Connect them at their mid-points and (2) make them Equal length.

As before I'm drawing these lines on the Construction layer (relations temporarily turned off so you can see the new lines):

The red bits are the end points of the new lines - they've been snapped to the mid points of the existing sketch. The green shows the mid points of the lines I want to Connect:

The two new lines connected at their mid points and made equal:

Bastard Child 22nd May 2011 1:36 PM

Dimensioning: To summarise a few key points about dimensions...

1) Place dimensions on a separate layer to the rest of the sketch
2) DRIVING dimension will set the length of a line (default colour black)
3) DRIVEN dimension will only report the length of a line (default colour green)
4) Lock symbol will toggle between modes OR,
5) Adding too many dimensions will default all new dimensions to driven
6) Set global settings for decimal places, font size, arrow size, etc. here:

One thing that craps me off is the use of comma delimiters in software and in general use around Europe. Set that shit to decimal, yo.

Example: Let's start with a really basic shape - here's a sketch we'd like to dimension, note we're going to place them on a new layer and use the ISO style:

After clicking the Smart Dimension tool you'll note the cursor turns any line under it Red to show what's being highlighted.

You can either left click a single line, or two end points on a line to define length! You're free to place the dimension anywhere on the page* with another left click:

* Pro's tip: Don't place a dimension inside a sketched object OR too close to an object because it's noobish. The following makes you look like a fucking idiot, especially when sending off a drawing for a professional to use:

You can move a dimension with the Select tool. Click the 'dimension line' (not the text) and drag it across the page:

The following two styles shows the difference between selecting a line, and selecting the end points of a line, when placing a new dimension.
-The dimension on the left is parallel to the line and is called an ALIGNED dimension
-The dimension on the right is horizontal, and called UNIDIRECTIONAL:

The vertical dimension placed here is also unidirectional (meaning it's showing a horizontal or vertical distance):

If you think the arrows should be on the outside (for clarity), use the Select tool and drag an arrow head to the outside of the 'projection line':

I'm going to delete the last couple of dimensions to show you Angle Between. Hit the tool and have a go placing angles on the page:

What we probably want though is the angle of a line with respect to a horizontal plane.

To do this I draw a line on the construction layer which can be made hidden, later:

Placing the angle down:

Hiding the construction layer:

You'll note I drew the construction line going to the left.

If you do it to the right the angle dimension won't get a 'projection line':
http://i20.photobucket.com/albums/b2...h_ff6c370a.jpg http://i20.photobucket.com/albums/b2...h_343808e1.jpg

Solid Edge REALLY dislikes two lines on top of each other... I'm sure you'll find that out when sketching!

Over-Dimensioning: The goal of dimensioning is to tell Solid Edge what size and shape to make the sketch. You CAN go overboard when dimensioning so pay attention to your work.

-In drafting, you want to show just enough information for someone to accurately recreate the sketch in a physical form. In modelling go with the same principal - just enough dimensions for Solid Edge to do its work.

Take a look at the following example:

Issue 1: We have a few dimensions appearing twice
-Do not clutter your sketch with unnecessary duplication:

Issue 2: If it looks 90[SUP]o[SUP] it can be assumed so!
-It's not necessary to show a 90 degree corner when it's easily inferred from the sketch:

Issue 3: Delete redundancy!
If two dimensions can be added (or subtracted) to find a third, don't include the third:

Same goes for right-angled triangles - math slap

Any of the following sketches are acceptable:
http://i20.photobucket.com/albums/b2...h_97894b8f.jpg http://i20.photobucket.com/albums/b2...h_4c0a172c.jpg http://i20.photobucket.com/albums/b2...h_fac17e0c.jpg http://i20.photobucket.com/albums/b2...h_f560b71d.jpg

So how do you figure out when you've got just enough dimensions? Let's go back to a more complex sketch and look at constraints...

Question to ask yourself - why would the bottom dimensions here be black (driving) whilst the right hand side dimensions be green (driven):

So, let's choose some random dimensions and size this bitch up...
-Overall sketch size 250mm x 250mm
-Thickness of arms 25mm
-Slot diameter 10mm by 20mm long
-Fillet radius 5mm

Check you're on the correct layer, select the Smart Dimension tool, check you've turned ON driving dimension, and start clicking random lines.

Edit dimensions by going to the Select tool and clicking the dimension's value (the text number):

What happens if you select an already dimensioned line and try and edit its length:
http://i20.photobucket.com/albums/b2...h_b88ef46a.jpg COMPUTER SAYS NO!

The problem here is that we're trying to lengthen a line that is already being controlled by a dimensional constraint.

So throwing dimensions down is constraining the sketch from moving around, just like using geometric constraints did earlier (equal, collinear, connect, horizontal, vertical, tangent, etc. commands).

So why is it we're getting green/driven dimensions on our sketch?:

Well, we have sketch with two intersecting lines that we forced into an Equal relation earlier. Dimensioning one of them is automatically setting the length of the other line - so one dimension is enough to constrain the sketch in both height AND width.

Let's delete our dimensions - Use the Select tool -> click anywhere on a dimension's leader line (but NOT the dimension's text box) -> press the keyboard delete key to remove it:

Now let's see how much freedom our sketch has to move around (or how many constraints we're missing):

7, huh? Now add a couple of Driving dimensions:

Now we're down to 5. Let's dimension the sketch with the numbers listed earlier and check it for unconstrained movement:

http://i20.photobucket.com/albums/b2...h_9d9ff040.jpg http://i20.photobucket.com/albums/b2...h_4047aba6.jpg

If you look carefully you'll see the shape of the sketch is fixed, so we're not missing any dimensions, it's just that the sketch is free to move on the page. If only we had an Origin to fix it to... oh wait:

By connecting the sketch to the origin we drew earlier (which is locked to the page), we've now fully defined it with no unconstrained movement:
http://i20.photobucket.com/albums/b2...h_307ec454.jpg http://i20.photobucket.com/albums/b2...h_78784de4.jpg

You can now save your work (and a copy as a DXF), or begin the drafting tute to make an A4 drawing with a title bar.

Bastard Child 22nd May 2011 1:36 PM

Advanced Sketching: In the sketch above - we started drawing our shape from one corner -> added new lines as we went around -> added construction lines and relationships -> then finished off with dimensions. It's a tried and tested method, and gives you a basic sketch.

Apps like Solid Edge have far more design power than you could appreciate at this point, young Padwan. In the previous sketch you saw the use of Equal geometric relations applied to force two lines to be the same length.

What if I wanted one line to permanently be 1/2 the length of another? Where's the tool for that?

What if I wanted the fillet radius to be 1/3rd the size of a line, but only up to 10mm max?

Let's take a brief look at some of the more powerful stuff which the majority of the great unwashed are ignorant of.

Example: We'll draw the same object as before, but I'll add a few rules...
Design intent:
1. Object shall be the same height and width: LENGTH = HEIGHT
2. The object shall be (mostly) symmetrical
3. The arms of the cross shall be 1/10th the size of the overall object: ARM WIDTH = 1/10 LENGTH
4. The slot's length shall be 5mm less than the arm's width: SLOT LENGTH = ARM WIDTH - 5MM
5. The slot's diameter shall be the difference between arm width and slot length: SLOT DIAM = ARM WIDTH - SLOT LENGTH
6. The fillet radius shall be 1/2 the slot diameter, but no smaller than 3mm and no larger than 15mm: 3 ≤ FILLET = SLOT DIAM ≤ 15

As before, start with an origin drawn on the Construction layer (or better yet, a layer called origin):
http://i20.photobucket.com/albums/b2...h_9a334b93.jpg <- I'll move this to a new layer called Origin, shown in the next picture

Sticking to the construction layer, I'm going to draw a cross of Equal length and height and joined in their middles with the Connect tool (Line type Center):
http://i20.photobucket.com/albums/b2...h_d884a7a4.jpg http://i20.photobucket.com/albums/b2...h_432cd3fc.jpg

Now when I draw my outline sketch, I can use these construction lines for mirroring. I'll add a few lines to my sketch as a starting point:

Mirror Tool: Use the mirror tool for making copies of a line (or a chain of several lines) around a datum - the mirror axis.

You have the choice to make a Copy of a line as you mirror, or to simply flip the line over the axis without leaving the original behind. We need the copy...

Start by selecting the tool:

Making sure Copy is enabled:

Dragging a selection box over the entire sketch:

Then clicking a line to mirror about:
http://i20.photobucket.com/albums/b2...h_0eb1e083.jpg <- right click to place object

You don't have to pick a line to mirror about, you can click any two points on your page.

Now grab a line and drag it around the page, watch how the other half of the sketch behaves:

When you Connect two points they'll met in the middle:

You could also have just drawn this basic shape first -> mirrored -> then joined them with a single line:

It has the advantage of using one less line. Something to think about at least.

At this point some of you may be tempted to mirror all the lines we have about a horizontal line, making the sketch below:

Add a fillet and see what happens:

Answer: Adding the fillet has broken the mirror relations. You have a choice...

1. You can either draw one half and mirror it as before:

2. Or you can force sketched lines (already drawn) to act like they're mirrored with Symmetric Relations.

Symmetric Relations: Found on the relationship toolbar this tool forces a line to behave the same as another, across an 'axis of symmetry'. Quick example...

Here I've placed 3 good lines on the left, and quickly drawn 3 lines on the right:

By using the Symmetric relation tool I can lock lines into behaving the same as those across the Symmetry Axis.

Click the Symmetric tool and pick a line to use for a symmetry axis:

Click on a line you want to be changed:

Lastly click on a line you want it to copy:

Easy eh?

So using mirror and symmetric tools we can get to this stage:

Add an arc and set its relations (tangent, etc.):

Mirror the bastard:

Then fix up the sketch with relationship constraints - here I've connected the sketch to my construction lines:
http://i20.photobucket.com/albums/b2...h_c169a6c3.jpg <- note that the right-hand arc doesn't need to be fixed as it's a mirrored copy of the left one

And an Equal relation:
http://i20.photobucket.com/albums/b2...h_afe92bd6.jpg <- note an alternative co-linear relation could have been used

Slot added, using one of the previous methods, and made Concentric with the arc on the arm:

You'll note I haven't yet made the four arms an equal width. I'll do this with a new method...

Bastard Child 22nd May 2011 1:36 PM

Dimensions and Variable Tables: If you can understand and make use of this topic, you're going to unlock some very powerful modelling techniques.

Every dimension you throw down is given a unique name by Solid Edge and put into a table. Checkout the following:
http://i20.photobucket.com/albums/b2...h_659317c5.jpg <- Grey means 'driven' (or 'display only')

If you double click a dimension you get access to this setting:

That sort of text - VXXXX is the default name given out. Why not give your dimension a useful name instead! You can't use spaces (or other reserved characters, probably):
http://i20.photobucket.com/albums/b2...h_c48ad243.jpg <- right mouse click to exit

Speaking of right-mouse clicks, you can choose to display all dimensions in terms of their name. Very useful for tracking down what name goes where:

We'll cover formulas in a minute. By default a dimension simply reports Distance, or how far apart its leaders (legs) are:

We can set up a table with numbers and formulas (the Variable Table) and as we dimension our drawing we're able to change the length of a line with a pre-made formula!

The following list is a copy/paste from earlier:

Design intent:
1. Object shall be the same height and width: LENGTH = HEIGHT
2. The object shall be (mostly) symmetrical
3. The arms of the cross shall be 1/10th the size of the overall object: ARM WIDTH = 1/10 LENGTH
4. The slot's length shall be 5mm less than the arm's width: SLOT LENGTH = ARM WIDTH - 5MM
5. The slot's diameter shall be the difference between arm width and slot length: SLOT DIAM = ARM WIDTH - SLOT LENGTH
6. The fillet radius shall be 1/2 the slot diameter, but no smaller than 3mm and no larger than 15mm: 3 ≤ FILLET = SLOT DIAM ≤ 15

Variables: Values, variables, formulas, limits, etc. are all entered into the Variables Table.

By default, the table simply lists what each dimension is reporting as its Distance value (this pic was shown earlier):
http://i20.photobucket.com/albums/b2...h_659317c5.jpg <- Grey means 'driven' (or 'display only')

If you have a sketch with no dimensions yet, the table will be empty:

We'll leave the Distance box alone - so that new variables (formulas) we add are going to be in units of 'mm'. If you click that box you'll see a drop-down list of other unit types like angle (degrees), mass (kg), etc.

The first thing we want is a variable to control the length and width of our sketch.
-Double click the first empty name box, enter a name with no spaces
-Double click the value box and put in a dimension, I've used 250
-Double click the comments box and leave a useful description

So our drawing now has a stored variable called LENGTH with a value of 250mm.

How can we make use of this?

Add a dimension to control the length (and width) of the sketch:

Now let's force this dimension to be driven by the variable we made called LENGTH:
-Double click the dimension's text
-Manually enter the variable's name into the formula box - LENGTH
-Click the green tick-box and right click the mouse to exit

Why the fuck can't you just click a drop-down box and easily select the variable name you want is beyond a fucking mystery to me.

So now if we bring up the Variable Table, we can see the following:
-The newly added dimension is called VXXXX (we can call it something more useful)
-The Value of this dimension is 250mm and is in a grey box (= driven dimension)
-The dimension is driven because its value comes from a Formula, and the formula says "copy whatever the value of LENGTH says"
-The dimension displayed on screen is green, indicating that it's not driving but driven

The above is also an alternate way to edit a dimension.

...and from now on whatever we type into LENGTH will change the size of our sketch:

The next screen is with all variables filled out according to design intent. Length is the only one that is not driven (locked):

The help file can help you with syntax and stuff:
http://i20.photobucket.com/albums/b2...h_a6bfadc3.jpg http://i20.photobucket.com/albums/b2...h_93d79d05.jpg

Now you can add dimensional constraints and link them to the appropriate variable:
http://i20.photobucket.com/albums/b2...h_bd552dea.jpg http://i20.photobucket.com/albums/b2...h_6a8ca737.jpg http://i20.photobucket.com/albums/b2...h_a365696a.jpg

...and doing that to the rest of the dimensions:
http://i20.photobucket.com/albums/b2...h_63270b86.jpg http://i20.photobucket.com/albums/b2...h_4899a566.jpg

So we have a fully defined sketch that works to an interdependent set of rules!
http://i20.photobucket.com/albums/b2...h_01b2bcd6.jpg http://i20.photobucket.com/albums/b2...h_4aafde39.jpg

Bastard Child 22nd May 2011 1:36 PM

For people sending off DXF designs for laser cutting, drafting your sketch isn't necessary. Just send a DXF of the model with a couple of important dimensions on it so the operator can check that it's scaled/cut to size properly :thumbup:

You can either delete all but a couple of key dimensions on your existing layer, or make a new layer called "Dimensions Laser Cut" and rename your old layer "Drawing Dimensions".


For a rough tutorial based on an old version of Edge: PDF warning
Here's what I'll typically use for A4 drawings - uploaded here

Drafting tends to give people the shits, and with good reason (I do it daily as part of my job). It's boring, it's tedious and some fucker will always find a mistaek on the page somewhere. If you want to draw to Australian Standards, search the for sale forum or ebay for A W Boundy's book - Engineering Drawing.

So at this point we have a complete model/sketch that's fully constrained, and it has dimensions and drawn lines placed on various layers.

This final topic will place that model onto a drawing sheet, scale it to fit onto the page, add a title bar with names/dates/titles/etc. and scatter some dimensions around the drawing.

Just on the topic of dimensions - CAD packages allow you to import model dimensions straight into the drawing sheet saving you effort. Alternatively you can also hide the model's dimension layer and dimension from scratch. I'll cover both topics.

Let's start by setting up a drawing sheet...

Generic Drawing Sheet: Click the tab at the bottom of the model window to switch to the drawing sheet. This is the typical sheet that Solid Edge 2D provides:

You can select the size of your drawing sheet (and choose to display the title bar and page borders) by entering Sheet Setup - method 1 via App Button, method 2 via right-click of Sheet 1:

You can add text to the title bar via the Properties screen (each box on your title bar is linked to that Properties screen). I've entered dummy numbers in each tab to see where it ends up in the title bar:

Custom Drawing Sheet: Let's face it the generic one is fugly and takes up far too much real estate. To edit the drawing sheet you need to enable the Background button and disable the Working button:

There should be a watermark on the page saying BACKGROUND to indicate that we're not doing regular drawings but modifying the page.

Experiment with the left and right mouse buttons to edit stuff and delete unnecessary lines. You can add company logo's and pics, and add your own text, and add HTML hotlinks (probably).

Make a new layer on the drawing sheet for the title block/text/page border if you wish.

Callout Screen: If you want your custom title bar to be automatically populated with names, dates, etc. you'll need to become familiar with the Callout screen. Here I've right-clicked the '3333' text that appears in the box for DRAWN NAME:

Pay attention. Whatever we type into the Files Property box (this thing):
http://i20.photobucket.com/albums/b2...h_488eafb0.jpg Go to the Summary tab -> Author

Will be displayed here:
http://i20.photobucket.com/albums/b2...h_c8c1a1fa.jpg See how the syntax is %{name}

Also valid:
%{Manager} ... or bring up the help file and search for "Property Text source list (Source: From Active Document)"

So now you can add a link from your document's 'properties page' to your title bar and not have to manually edit your drawing's name etc.

To make your own callout textbox from scratch click Callout -> enter your text and modify font, size, etc. -> click ok to exit screen -> TURN OFF ARROW -> place text on page with left click:
http://i20.photobucket.com/albums/b2...h_7ad0edd8.jpg http://i20.photobucket.com/albums/b2...h_87d40ceb.jpg

I don't know of a way of easily aligning multiple text boxes together like other programs do. I just draw a horizontal line and carefully move text around so it's manually lined up.

Here's what I'll typically use for A4 drawings - uploaded here:

Example Drawing: With the A4 sheet open, let's insert a model and scale it.

Find the 2D Model button which will take you to the 2D model page:

Here we drag a selection box around the 2D sketch which will crate a 'viewing window' that links the 2D model through to the A4 sheet:

After we've placed the second click we'll get to choose where to place the sketch on the A4 page. I've left the scale 1:1 so you can see how large this sketch is in relation to the paper:

So the model is clearly larger than an A4 sheet. We *could* create an A3 sheet but I'll scale this model down to 1:2 (i.e. 1/2 scale).

Click on any line to highlight the model, then find the Select Scale box:

It now fits!

Note that the scale is bloody wrong! Obviously the callout text box isn't reporting the drawing's scale but probably the A4 sheet (don't ask). Let's fix it now by changing what this callout is linking to.

Enter Background mode for the A4 Sheet to unlock the title bar for editing -> right click the 1:1 text box and bring up its Properties:

Change Sheet Scale to something else, say, Category:

Now you can manually change the scale to the correct value:
http://i20.photobucket.com/albums/b2...h_aae92fbb.jpg http://i20.photobucket.com/albums/b2...h_1379ccc3.jpg

If you have downloaded my A4 template file, this is something you'll want to fix and save.

Return back to Working view and the A4 sheet:

At this point we can make changes to the Drawing View like hiding layers that we don't want printed or displayed:
http://i20.photobucket.com/albums/b2...h_8721f09b.jpg <-Note that 2D Model still has Construction layer turned ON, it's only on the A4 drawing page it's hidden

Dimensioning: I'm not here to teach you to draft and annotate to Australian Standards 1100, but how to use Solid Edge tools competently (buy an A.W. Boundy book if you want).

Start by hiding layers in the Draft folder (red) so just the outline of the sketch is being displayed. I've created new layers for my centrelines and drafting dimensions (green):

Dimension Style: Up to this point we've been using the standard (or a slightly modified) ISO style for dimensioning our 2D model:

Now that we're in the drafting sheet environment we should set up a unique dimensioning style for a couple of reasons...

1) Sketching out a 2D design involves a lot of page zooming and panning. It's handy to have a nice large font for clarity (10mm say). When you switch to drafting, a large font takes up too much space and makes your drawing look amateurish - you'd want a reasonably small one (3-5mm say).

2) Any dimensions we place on the A4 drafting sheet are going to end up green (driven dimension style):

This happens because the model is already fully defined on the 2D Model page with dimensions and relationship constraints. Any new dimensions we place on the A4 drafting sheet will default to driven.

Solid Edge will not let you place 2 driving dimensions to control the same line.

So let's create a new ISO style (based off the original) and modify it as so:
-I've called it ISO Draft
-Driven colour made black
-Font size changed to 3mm

Just a quick note on the way Solid Edge behaves - when you insert a 2D sketch and scale it to fit onto your drafting sheet, Solid Edge will ask if you want any text automatically scaled or left its original size. I don't care as I make my own style as shown above.

Center Mark: Placed on my Centre layer, use center marks to indicate hole and fillet/round centres. I don't use the default style:

Here I've applied marks to the slot and only one fillet:
-Check you're drawing on the correct layer
-Double check you're using ISO Draft style
-Turn Projection Lines on or off with the circled icon

I've only centre marked one fillet, the other will get a dimension arrow placed there so a centre mark may clutter things.

Key Points: Drawing notation is difficult to do well - it's an art and everyone does it a bit different. This also means I can't give you hard and fast rules for every situation. Have a look through this website (hit next page found top-right) and check google image for 'dimensioning'.

Guidelines from post #3
-Don't place a dimension inside a sketched object OR too close to an object
-You want to show just enough information for someone to accurately recreate the sketch
-Do not clutter your sketch with unnecessary duplication
-It's not necessary to show a 90 degree corner when it's easily inferred from the sketch
-If two dimensions can be added (or subtracted) to find a third, don't include the third
-A dimension parallel to a line is called an ALIGNED dimension
-A dimension that's horizontal or vertical to the page is called UNIDIRECTIONAL

In summary don't over-dimension, keep it to a useful minimum.

Here's our model with dimensions added to the correct layer, and with the correct style used:

I try and use a dimension style suited to the manufacturing process used to make that part, and I try and dimension it to account for the performance of the equipment used.

A LASER cutting beam used by one of my suppliers eats between 0.1mm and 0.4mm of material (depending on a number of factors). If I ask for a 6mm hole in a piece of steel it could end up as small as 5.6mm, or as big as 6.4mm, depending on which side of the drawing line the beam ran along, LASER power, running speed, material type, thickness, etc.

If I wanted a hole very close to 6mm - say 6mm 0.05 I'd get the LASER dude to cut a hole 5.5 and I'd finish the job with a fresh drill bit on a press.

Have a chat to the guy making your part so you're each clear on what's required and what limitations you're both working with.

Let's say our shape is going for LASER cutting. The operator will likely have a steel ruler and vernier/calliper handy. If I provided the following three drawings, which do you think he'd find easiest to work with?

1. http://i20.photobucket.com/albums/b2...h_af42beec.jpg

2. http://i20.photobucket.com/albums/b2...h_0ed6013a.jpg

3. http://i20.photobucket.com/albums/b2...h_8bb1cc15.jpg

Drawing 1 would involves finding a part's centreline - easier to do in CAD than in practice especially where accuracy is required. Try and avoid these types of dimension placements.
-What if I asked you to find a centreline to an accuracy of 0.01mm but you only had a ruler graduated every 0.5mm?
-If I gave you a pipe and asked you to find the radius, you'd measure the DIAMETER and halve it. So why bother listing radius dimensions to a fitter and turner...

Drawing 2 involves three measurements, but is really saying - I don't care what the width of the arm is as long as the other measurements are ok. Nothing wrong with that, but it doesn't let you easily see what the arm's width is.

Drawing 3 looks to be the easiest one to work with. You'd measure the overall length of the object, then the arm's width. It's assumed the arm is centred on the part hence we don't bother detailing how far the arm is from any edge.

A drawing like this just screams noob

Detail View: This is typically used to place a 'zoomed in' view on the same sheet as your drawing (I'll keep this very brief because I doubt most of you will use it).

Let's say we want a better view of the slot. Navigate to the Detail button:

Choose a shape for the view port, a scale, and click on the drawing sheet to select what area you'd like zoomed in:

Place the Detail View on the drawing sheet:

Note that you can hide layers in that view (turn off dimensions and make your own for example), you can click (or double click) the detail view and change the border size, scale etc.

Bastard Child 22nd May 2011 1:36 PM

Sheet Metal Bend Calculations: Before we get into bend calculations, you should have some idea of what's involved in bending sheet metal. Watch the following vids:

Electrabrake/Magnabend holds one side of the work piece firmly and flips up the other side:

^- At work we bend up to 2.5mm stainless and 3-4mm mild steels (~3" width in either case). For you guys designing mobo trays or cases you'll easily do 1-2mm thick panels in mild steel or aluminium (x 1m wide).

Thicker material needs larger forces, typically this is done on a press brake. Note how the bend forces both sides of the materiel 'up' - skip to 1:40 in first vid

Then you have machines like a pan brake which is similar to a Magnabend, but with mechanical clamping - skip to 6:20


From here on out I'll only be referring to bends made by a Magnabend type machine, it's what I use at work and am familiar with. Here's the basic parts:

1. Clamp Bar - This wide piece of steel will clamp down onto the table when electricity is applied through the table's electromagnets. It can be adjusted forward/back by a screw to set the bend radius before you begin
2. Table
3. Bending Beam - This piece swings up on a hinge and the handle has angle markings on it
http://i20.photobucket.com/albums/b2...h_976e8a4e.jpg http://i20.photobucket.com/albums/b2...h_ac006152.jpg

Here's a close-up of what's happening in the bend area:

As the bending beam swings up it forces the sheet to bend from the sharp edge of the clamp bar. When talking about 'bend radius' with respect to a magnabend type device we are referring to the OUR RADIUS. I'll repeat:


This is important to remember as our calculations will be using INNER RADIUS. Fuck this up and I'll come to your house and shit in your dishwasher - you have been warned.

As mentioned somewhere above, to adjust the bend radius the clamp bar is moved forwards or back before bending (you can typically adjust outer bend radius from 0 to 2.5mm):
http://i20.photobucket.com/albums/b2...h_1c75deeb.jpg <- By moving the clamp bar back, we've given this sheet a larger bend radius (both inner and outer).

So what? Who the fuck care about bend radius? Why the fuck can't I just bend my shit with a sharp corner?

To answer those questions you need to understand what happens to a material as it gets bent.

Bending Stress And The Neutral Axis: When you bend a material over in a tight curve you're actually squashing the inside and stretching the outside fibres (or metallic grains).

That also means that somewhere inside the material it's neither being squashed or stretched, but it remains at its original length:

Important Note: If we bend our sheet too tightly (make the bend radius too small) the sheet can crack as the tensile forces on the outer surface tear apart the structure of the material.

As a general rule keep the INNER bend radius 2-3 times the thickness of the sheet. The thicker your material, the larger the bend radius will have to be. Speak to your fabricator about material selection and minimum bend radius.

By definition the neutral axis will not undergo a change in length during deformation:

^ I've drawn that neutral axis about halfway through the sheet. In reality it depends on how soft/hard the metal is and what type of bending method is used - typically the neutral axis exists 30% - 50% from the top surface (this is called the 'K-factor', 0.3 to 0.5).

While I used the Solid Edge SMART DIMENSION tool to find the length of my bend (a perfectly valid method), if we know how deep this neutral axis is inside the material, how far the sheet is bent, how thick it is, what bend radius is used... we can calculate how much sheet it takes to form the bend!

Why do we care how much sheet metal it takes to form a bend? Glad you asked...

1. Bend Allowance: This calculation will tell you how much metal is used to form a bend:

Bend Allowance = A (Pi/180) (R + K x T)

Bend Allowance = length of arc needed to form bend (mm)
A = angle of bend as drawn in picture (degrees)
K-factor* (t/T) = depth of neutral axis (no units because mm/mm cancel out)
T = sheet thickness (mm)

*K-factor can be obtained from bend tables like this one on wiki

Most of the stuff I bend is steel, with an inner bend radius equal to or a bit larger than thickness. I use K=0.45 for all my jobs:

When you've worked out how much material is required to form a bend you'll then be able to work out how much overall metal to cut, and where to bend it!

Example: Let's take a 1mm piece of mild steel, mark a pencil line 20mm from one edge, and bend it 500 with the magnabend set to R=2.5mm:
http://i20.photobucket.com/albums/b2...h_22adfd31.jpg http://i20.photobucket.com/albums/b2...h_a04a87f9.jpg


With the pencil mark lined up with the edge of the red clamp bar, can you see the bend will occur between the pencil mark and the 20mm edge:

So how much material is used around the bend?

Bend Allowance = A (Pi/180) (R + K x T)
A (angle of bend) = 500
T (sheet thickness) = 1mm
R (INNER RADIUS = outer radius - sheet thickness) = 2.5 - 1 = 1.5mm
K-factor = 0.45 from here

BA = 50 (3.14/180) (1.5 + 0.45 * 1) = ~1.7mm

To check, here's a drawing of the bend:

So our calculations say the bend allowance is ~1.7mm, leaving us with a flange of length 18.3mm (20-1.7). We now have a way of calculating how much material is used to produce a bend.

Example 2: You want to make the following object with two holes, where the crap do you draw them with respect to the bend line?:

Before we do any calculations, let's study what's going on. Here's the bottom hole:
I hope it's obvious that it doesn't matter what the bend radius is, the hole will always be located '12-R' away from the bend line.

Here's the r.h.s. hole:
It's easy to find the distance of the hole from the black line that marks the end of the bend: 15 - ( R + T)

But that only tells us how far the hole is from the 'end' of the bend. How far is the end of a bend from the beginning? It's the bend allowance figure we learnt how to calculate, DUH!

Let's use the following data for our example - with the magnabend set to R=1.5mm:

Bend Allowance = A (Pi/180) (R + K x T)
T = 1mm steel
R (INNER RADIUS = outer radius - sheet thickness) = 1.5 - 1 = 0.5mm
A = 900
K = 0.45 (you could also use 0.4 for bends smaller than T)

BA = 90 (3.14/180) (0.5 + 0.45 x 1) = ~1.49mm
http://i20.photobucket.com/albums/b2...h_1d7b60e4.jpg <- our bend will chew up ~1.49mm of material

1. Right hand side hole, distance from bend line: 15 - (R + T) + BA = 15 - 1.5 + 1.49 = 14.99mm :thumbup:
2. Bottom hole, distance from bend line: 12 - R = 12 - 0.5 = 11.5mm :thumbup:

Now locate your intended bend line with respect to a sheet edge and you're set :thumbup:

2. Bend Deduction: If needed...

BeanerSA 22nd May 2011 1:39 PM


Originally Posted by Bastard Child (Post 13215900)
Do people want more or is it over everyone's head?

These things are handy, and it will always strengthen your own understanding. Keep it going. Why this though, and not 3D drafting in SketchUp?

Enjoi 22nd May 2011 3:32 PM


Originally Posted by Bastard Child (Post 13215900)
reserved 2.

Drafting space.

Do people want more or is it over everyone's head?

this is awesome dude, as much info as u can put here the better i say, im sure us modders that want to take our modding one step further will surely appreciate this!

+1 rep to u sir :D

AlastairT 22nd May 2011 3:40 PM

You're a legend, mate. There's certainly a need for a nice, simple introduction to a decent free CAD program, given the number of people that want laser cutting/CNC milling done.

slattzZz 22nd May 2011 4:28 PM

:thumbup: Superb thread mate, keep it coming if u could be arsed, I will definitely add this proggy to my modding arsenal on my build: SG-PC.

Recently spent hours modeling designs in SketchUp, then my plastics fabricator tells me he'd prefer 2D design drawings!!

gruntLOL 22nd May 2011 5:12 PM


Originally Posted by BeanerSA (Post 13215907)
These things are handy, and it will always strengthen your own understanding. Keep it going. Why this though, and not 3D drafting in SketchUp?

Because if you ever want to outsource the work to get it made by someone they will tell you to come back with 2D flat panel layouts for most things. If it needs to be folded or formed they'd still rather the flat layout and the folding info than a 3D model, they are a pain to measure and most software won't be able to replicate that for CNC work.

Sketch Up is only good to make sure things are all going to fit, but the same can be achieved with 2D stuff and a ruler.

EDIT: Nice work on the tutorial hopefully it will help out a few people here that need to get stuff done.

broox 22nd May 2011 10:45 PM

I've been thinking about getting some 2d software and designing some things to be cnc/laser/watercut, and ultimately for folding up :thumbup:

heaps usefull, picked up a few tips and answered a few small questions from just a quick glance. will definitely be using your guides and that program :thumbup:

Enjoi 25th May 2011 7:26 PM

Hi bastard,

just went through your tut tonight and found it a lil hard to follow :S

as a complete noob, im having trouble making things look the same as what you have in your pictures, which is what im using as checkpoints to make sure im doing the right thing.

is there any way u can be a little bit more step by step with your info?

cheers buddy,


Enjoi 25th May 2011 9:05 PM


Originally Posted by Bastard Child (Post 13228632)
Chillax, I haven't begun the drawing part yet :thumbup:

As people will see I'm doing bits of the drafting tute at the moment.

all good dude, i sincerely appreciate it! just saying that some of the drawings in the first section with the angles displayed and such, makes its a bit confusing when i dont know how they got there lol

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