After creating all required views on the drawing sheet, applying dimensions, creating parts and assembly numbers along with relevant annotation, tolerance, machining symbols, welding symbols etc. is the next logical step in creating drawings. We will see how we can apply these.
Creating balloons
Having an exploded view in drawing along with part numbers in balloons can help parts assembly process. Creating it is also easy, however, you should have the parts positioned in the location in the assembly environment and create that view in drawing. After creating the view, you may want to isolate that view since updating the part / view would disturb the drawing. Before we generate balloons, you may want to modify a few settings using the path Tools > Options > Mechanical design > Drafting > Generation tab and Annotation and Dress-up tabs.
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| Setting for number generation for all instances |
From the generation tab, you can choose if a part is used repeatedly in an assembly, whether each instance should be applied a balloon.
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| Setting for balloon numbers |
And from the annotation and dressup tab, you can decide if the balloons created should be numbering, instance name or part number. After you have done the settings, you can easily create the balloons by using the path Insert > Generation > Balloon generation.
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| Generating balloons |
Either you can create dimensions automatically by utilizing the constraints that you used to create parts, assemblies or you can apply dimensions using the dimensioning toolbar.
Automatic
The automatic method can be used to generate dimensions of the parts as well as assemblies. There are a couple of customizations that you should know before you go on to generate the dimensions automatically. These settings can be opened using the path Tools > Options > Mechanical design > Drafting > Generation tab. In this tab, you will find the option "Generate dimensions from parts included in assembly views", the option is unchecked by default, since it is unlikely that you would require to generate part sketch constraints if you are creating a drawing from an assembly. However if you check this, you will be able to add / select parts of an assembly while generating constraints for views generated from an assembly.
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| Customization options |
You can also set the "Delay between generation for step by step mode" from the same tab, this will come in handy too when we are generating dimensions using the step-by-step method.
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| To enable generated dimensions to drive 3D geometry |
By default, automatically generated constraints cannot drive 3D geometry, however you can change this setting from the Administration tab and drive 3D geometry using the generated dimensions. There are two ways in which you can generate the automatic dimension:
- Generate dimension
- Generate dimension step-by-step
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| Generate dimensions dialogue box |
- Sketcher constraints - These are constraints that you applied to constrain a sketch.
- 3D constraints - These are constraints that you where you created a reference plane using offset distance from a plane etc.
- Assembly constraints - Constraints applied in an assembly. (Available when you created drawing views of an assembly).
- Measured constraints - Any reference constraints created in a sketch.
You can choose among options from - Generate dimensions from constraints
- associated with unrepresented elements - This will create constraints even if there is not an appropriate visible element in a view.
- with design tolerance - If you applied tolerance with constraints while making a sketch and want to generate those tolerances too along with dimension, you can do it using this option.
Catia keeps a track of dimension that you do not want to create. The option 'Retrieve excluded constraints' will be available when you choose to generate dimensions the second time or on any future attempts to create dimensions. And any dimensions that you deleted while creation process ran previously, these dimensions can be retrieved using this button and you can generate them too.
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| Dialogue box for step-by-step generation |
While the dimensions are getting generated, you can choose to not generate them by using the button, 'Not generated' and can even transfer them to an alternate view using the button 'Transfered'. If you tile windows horizontally or vertically, you would also be able to use the visualization in 3D option and see the dimensions that are getting generated.
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| Analysis dialogue box |
After the dimensions are generated, you can analyse the dimensions that are generated. You can switch back and forth between part window and drawing window and analyse them to see generated constraints, generated dimensions etc.
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| Using Generate dimensions step by step |
Above you can see that we are generating dimensions step by step of a cup designed in Catia. The views were already put on the drawing sheet. You can see that we selected the option "with design tolerances", so this will apply dimension tolerances wherever we had them in our sketch constraints. Also, the option "associated with dimensions with unrepresented elements" is chosen so that we can get dimensions even if the represented element is not present in view. Since it is a part for which we are generating the dimensions, the type of constraints option "Assembly constraints" is greyed out.
Dimensioning toolbar
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| Tools present in Dimensioning toolbar |
The tools in the dimensioning toolbar are dimensions, chained dimensions, cumulative dimensions, stacked dimensions, length / distance dimension, angle dimensions, radius dimension, diameter dimension, chamfer dimensions, coordinate dimensions, hole dimension table, coordinate dimension table, re-route dimension, create interruptions, remove interruptions, create / modify clipping, remove clipping, datum feature and geometrical tolerance. Most of these are self-explanatory and you can use them by simply selecting circle, lines etc. and the dimensions will be created. In case of all of these, you get more options the moment you right click while you are in the dimension creation mode.
Dimensions
The tool is versatile and can be used to apply dimension of a line, distance between lines or points, curve length, point coordinates, angle between lines, radius, diameter etc.
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| Applying all sorts of dimensions using just one tool |
Additional options are also presented in the tool palette that you can use to force vertical or horizontal dimensions. Above you can see that a single tool was used to create, length, distance, angle, arc length, diameter and point coordinates in a drawing. So using this you can create almost all types of basic dimensions.
Chained dimensions
As the name indicates, you can use this to create chained dimensions. It is the type of dimensioning where the end point of previous dimension acts as start point of the next dimension.
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| Creating chained dimensions in Catia |
This type of dimensioning increases accumulation of tolerance error. Above you can see we created chained dimensions, also used the tool palette to force vertical dimensions.
Cumulated dimensions
The cumulated dimensions are much like stacked dimensions, however they differ in the format.
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| Creating cumulated dimensions |
In a sense it can be said that cumulated dimensions are a combination of chained and stacked dimensions.
Stacked dimensions
The stacked dimensions use same starting point for all dimensions and this eliminates the chances of tolerance error accumulation.
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| Creating stacked dimensions |
Length / Distance dimensions
This can be used to used to apply dimension on a line, measure distance or measure arc lengths.
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| Applying arc length dimension |
You can access relevant options related to the tool using a right click.
Radius dimensions
The tool applies radius value on the arc or circle that you select. Additional options can be accessed using right click, as we do in this case.
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| Creating radius dimension |
Diameter dimensions
The tool will apply diameter value to the arc or circle that you select, much like in case of radius dimension.
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| Creating diameter dimension |
Chamfer dimensions
If you have applied chamfer in your design, you can dimension it using this tool. There are various ways in which you can dimension it. This is much like the different ways in which the chamfer can be modeled. To create the chamfer dimension, you will need to select the chamfer edge.
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| Applying chamfer dimension |
Chamfer detection will point out the order in which it is making a selection. 1 indicates the edge that is dimensioned, while and 2 and 3 indicate the first and second reference edge respectively. By moving the cursor, you can switch the order i.e. 213 or 312 to have reference edges as you prefer. You can select the chamfer dimension type to be applied from the tools palette i.e. length and length, length and angle etc.
Thread dimensions
Visible threads in a drawing can be dimensioned using this tool. In case the threads are not visible, you can modify the properties and first mark them as shown from the dress-up section of the view properties as we have done in this case. Also, for the other view, we marked to show hidden lines as well as thread.
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| Applying thread dimension |
Coordinate dimensions
The tool can be used to dimension points in a drawing. The points coordinate will be created with reference to the planes position in the part. By default, the points that you create in a sketch or using reference elements will not be projected in a drawing.
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| Creating coordinate dimensions |
However, you can change this in the settings. Tools > Options > Drafting > View tab. In the Geometry generation / Dress-up section select the option Project 3D points.
Hole dimension table
To dimension series of holes, you may use a hole dimension table. A hole dimension table can be generated for holes to indicate position and dimensions.
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| Creating hole table |
Coordinate dimension table
Instead of generating coordinates for individual points and dimensioning them separately like we did in coordinate dimensions, you can instead generate a coordinate dimension table.
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| Creating coordinate dimension table |
Relevant text, machining symbols, geometrical tolerances etc. wherever they are required, for this we use the tools that are available in annotation toolbar.
Re-route dimension
In case you modify parts, or edit some feature of part, the dimension associated with part can lose association with edge using which you applied a dimension. Such a dimension will be shown in pink colour when you update the drawing.
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| Re-routing dimensions not updated after chamfer application |
Rather that recreating the dimension, you can re-route or re-associate the existing dimension with the edges of your choice. Above you can see how it's done.
Create interruption
You may encounter situations where the extension lines cross dimension line or other lines. In this case, to bring clarity you can create interruptions in the extension line of any dimension. First we select the extension line, second we create the first point of interruption and then the second point of interruption to be created.
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| Create interruption |
Above you can see we create interruption in one extension line of the dimension that measures 6 unit. If you wish to create interruption on both the extension lines, you can choose this from tool palette. If you wish to create multiple interruptions, you can repeat the command again.
Remove interruption
To remove an interruption, we may use this tool. We may chose to remove interruption on one side, on both sides or all interruptions, these options are available in the tools palette.
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| Remove interruption |
Create / Modify clipping
This tool is for dimension line, while interruption was a tool for extension line. This can be used to create or modify clipping of a dimension line. This can be used to clip one side of the dimension line as you prefer.
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| Clipping a dimension |
First we indicate the dimension to clip, then the side to keep and then the clipping point. The clipped dimension will turn orange, indicating that it's a clipped dimension. You can use the tool again on the same dimension to modify the clipping. Also, the tool can be selected to clip multiple dimensions together.
Remove clipping
To remove the clipping, we would use this tool. This will basically reset the dimension to original state.
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| Restoring dimension, removing clipping |
Annotations toolbar
The annotations toolbar has some tools that we need for writing text on our drawing or creating welding symbols, indicate roughness, balloons etc.
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| Tools in annotation toolbar |
Text
The tool can be used to write text wherever needed. You can also copy and paste the text box to place it wherever needed using the commands Ctrl+C and Ctrl+V.
Text properties toolbar
Text font, size and other properties can be modified using text properties toolbar. The toolbar can modify the text everywhere i.e. of dimension, text, text with leader, balloon etc.
Text with leader
Text with leader will first allow you to position the arrow, then you can select the position where you wish to place the text. Subsequently, the box appears where you can write text.
Text replicate
We can use an already linked text with some attribute of the part to readily make more such copies using text replicate. So, it involves first creation of text and linking it to some attribute of our preference. In this case, we link the text with hole diameter. Next, we create a copy of that text corresponding value of the attribute that we have preselected in the part.
We can use an already linked text with some attribute of the part to readily make more such copies using text replicate. So, it involves first creation of text and linking it to some attribute of our preference. In this case, we link the text with hole diameter. Next, we create a copy of that text corresponding value of the attribute that we have preselected in the part.
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| Using text replicate for hole diameter |
Above you can see we first added text 'Diameter value' and associated it with hole diameter. Next, we replicated the text and these were associated with other hole diameter.
Balloon
Datum target
A datum target is used to specify point, line, area on part so as to establish datum. This tool can be used to specify such points, areas etc.
Roughness symbol
Specific machining processes can achieve certain tolerance values, surface roughness value can be specified using this tool.
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| Creating roughness symbol |
Using this tool, we can specify if material removal is allowed or not, surface pattern information etc.
Welding symbol
Information related to welding can be put with welding symbol tool. With the dialogue box that opens up, you can specify if it's fillet weld, spot weld, plug weld or any other type of weld.
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| Creating a welding symbol |
In addition, you can specify complimentary information like whether it's a weld with flat face, convex face etc.
Weld
This tool can be used to specify a welding symbol that represents the kind of weld that you want. While welding symbol may communicate everything related to the weld. You can see above the black portion area was created using this tool.
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| Creating weld region using weld tool |
Welding symbol may represent the edge clearly where the weld need to be applied along with the desired shape. You need to select the edges between which this symbol needs to be created.
Table
If you want to add any table, you can do so using this tool. You would be able to define the number of rows and columns that you want, and edit it much like you do in Microsoft Excel.
Table from CSV
The CSV stands for comma separated values. You can also bring in table in the .csv format to the drawing directly using this tool.
Dress-up
Dress-up toolbar has a variety of features that can be used in case of interactive drafting i.e. where you have created drawing by yourself. It also has tools that come handy even in case of automatically generated drawings. The tools are Centre line, Centre line with reference, Thread, Thread with reference, Axis line, Axis line and Centre line.
Centre line and Centre line with reference
Centre line as the name tell us, can be used to create a centre line of a circle, ellipse etc. If you use the option Centre line with reference option, you can select a circle as reference or even a line as reference to align the centre line according to reference. Note that centre line with reference will not work with ellipse.
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| Creating centre line and centre line with reference |
Above you can see we create a centre line of a circle and centre line on circle with circle and line as reference.
Thread and Thread with reference
Thread and thread with reference works in the same way as centre line. However, in this case you get the option to choose from the tools palette, whether you are applying a thread or tap.
Axis line
Axis line can be created with the help of two lines, two circle etc. All you need to do is select the elements that you wish to create an axis line.
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| Creating axis line using circles and lines |
Axis line and Centre line
The tool can be used to create centre line of a circles etc. along with an axis in just one step.
Area fill creation and Area fill modification
If you create a section view from a part or an assembly, the hatch area will be automatically created. However in case you wish to create a hatch fill or colour fill, you can also use the area fill creation tool to fill an area with hatch pattern etc.
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| Area fill creation |
To select the area, you can either select all the edges manually i.e. with option Profile selection in tools palette toolbar or you can select using Automatic detection option. There's also an option to select / de-select Create datum option. With the use of Create datum option, the pattern fill will not modify if area changes. However, if you create it without the option, the hatch area will be dynamic and will change as the area changes.