Additional Tools of the CAM Editor in Altium Designer

Created: февраля 08, 2023 | Updated: февраля 08, 2023 | Applies to versions: 23, 24 and 25

Altium Designer's CAM editor includes a number of tools facilitating the execution of certain tasks when working with a CAM document.

Copper Area Calculation

To calculate the total copper area for selected objects in the current document, choose the Tools » Calc. Copper Area command from the main menus. After launching the command, the cursor will change to a small square and you will enter copper area calculation mode. The procedure involves the following sequence of actions:

Click on objects you wish to include in the calculation, making them selected. Clicking away from an object allows you to drag a selection area, for including multiple objects in the selection. Selection is cumulative.
Once all required objects have been selected, right-click. A report file (Copper Area.rpt) is generated and opened as the active document in the main design window. For each layer that is associated with the selected objects, the report lists the area of copper that will be used, in square inches. The total copper area is also listed.

The report is generated and saved automatically in your PC's \Users\<ProfileName>\AppData\Roaming\Altium\Altium Designer <GUID>\CAMtastic folder. To access the folder, right click on the report file (*.rpt) in the Projects panel and select the Explore option from the context menu.

Placing a Copper Pour

To fill a closed boundary with copper, choose the Tools » Copper Pour command from the main menus. After launching the command the cursor will change to a small square and you will be prompted to select a closed border. Closed borders can be circles, rectangles, or polylines (if they have been closed). The procedure involves the following sequence of actions:

Simply position the cursor anywhere over the border of the area you wish to fill with copper and click. The Copper Pour dialog will appear.
The dialog shows a preview of the pattern that will be used for the copper pour, and also a clearance value. This value provides a clearance boundary to ensure that the pour is contained completely within the bounds of the original image. By default, the last pattern for the copper fill to be defined, will be the one now offered. Should you wish to use a different pattern for the fill, click the Edit Pattern button, to open the Edit Pattern - Copper Pour dialog. Use this dialog to define the pattern for the pour as required:
1. If the Fill Type is set to Polygon (Raster), then all other settings in this dialog will be disabled. The selected boundary will be filled with a solid polygon and in accordance with any clearance specified in the Copper Pour dialog.
2. If the Fill Type is set to Vector, you may choose between using a solid image or a shape/Dcode. You can choose a shape and enter a size to use for the fill, or you can specify to use an existing aperture. If you have chosen to use Shape/Dcode, you can specify the XY spacing of the shape used.
After defining the pattern and clearance as required, click OK to pour the copper into the boundary.
Continue selecting further closed boundaries for pouring copper, or right-click, or press Esc, to exit.

Using a polygon fill will cause a new Dcode to be added to your apertures list. This appears as the entry Poex.
If you use shapes and sizes for vector fills that are not existing apertures, they will be added to the apertures list with the next available Dcode.
While a Polygon (Raster) fill appears the same as a Vector (Solid), it will be defined by large overlapping shapes rather than minute fills. This will generally keep the file size smaller and allow faster redraws.
Only positive values are accepted for the boundary clearance. Any negative numbers entered will result in the negative symbol being ignored.

Pad Removal

To remove isolated and stacked pads from all internal signal layers in the current document, choose the Tools » Pad Removal command from the main menus. After launching the command, an information dialog will appear, providing a summary of the isolated and stacked pads that were detected on all internal signal layers found in the current document. After clicking OK, the indicated total number of pads will be removed.

One or more layers in the current document must be of type Internal in order for this command to be used.
If using Altium Designer's PCB Editor to generate the Gerber files, disabling the Include unconnected mid-layer pads option - on the Layers tab of the Gerber Setup dialog - will effectively provide the same action as this command.

Modify Object Spread

The Tools » Spread/Reduce command from the main menus is used to increase or decrease the spread of a selected object, essentially adding thickness to, or thinning out the original aperture related to the object, and subsequently saving this as a new aperture.

After launching the command, the cursor will change to a small square and you will enter spread/reduce mode. The procedure involves the following sequence of actions:

Select the object(s) that you wish to enlarge/reduce. Simply position the cursor over individual objects and click to add them to the selection, or use one of the many selection tools available.
After all objects are selected, right-click. The Spread/Reduce Size dialog appears. Use the dialog to specify a size for the enlargement/reduction, making sure to include a negative sign when reducing. You can choose to have the new objects placed on the same layer, a new layer, or one of the existing layers. The Delete Old Objects option gives you the choice of keeping the original objects for comparison purposes.
After the sizing options are defined as required, clicking OK will effect the size change for the selected object(s). The resulting shapes that are obtained will be added as new aperture definitions - one per different initial aperture in the selection - and Dcodes will be assigned to each, starting at the first available (empty) Dcode.
Continue enlarging/reducing further objects, or right-click, or press Esc, to exit.

If reducing the size of an object, and the same layer has been chosen to place the new object, the Delete Old Objects option must be enabled, otherwise nothing will happen.
The new aperture definitions can be viewed from the CAMtastic panel, or in the Edit Apertures dialog (Tables » Apertures).

Teardrop Selected Pads

The Tools » Teardrops command from the main menus is used to teardrop selected pads on routing (signal) layers in the current document. Teardropping pads is a common technique for guarding against drill breakout during the board fabrication phase.

First, ensure that the routing (signal) layers that you wish to add teardropped pads to, are turned ON in the Layers list of the CAMtastic panel.

After launching the command, the cursor will change to a small square and you will be prompted to select the pads you wish to teardrop. Simply position the cursor over individual pads and click to add them to the selection, or use one of the many selection tools available. After all pads that you wish to teardrop are selected, right-click. The Add Teardrops dialog appears.

The left half of the dialog allows you to define the style of teardropping you wish to apply - either Pad or Line. The Pad style teardrop will place a pad, half the size of the original pad, at the trace/pad intersection. The Line style teardrop will place two lines (tangential to the pad) to fill in the trace/pad intersection. When using the Line style, you can specify a Line Offset Factor, which controls the length of the teardrop.

The right half of the dialog allows you to define and apply various clearance checks. Define these constraints as required. By default, each is set to 5mil.

The Inflate Pads/Vias bounding Rect By field is used as a method of speeding up the teardropping process. By inflating the bounding rectangle of a pad, you can narrow down the number of traces to be considered for teardropping to only those that touch the inflated boundary. Think of this as a coarse check, followed by the fine check of those traces that are left, to determine if they truly connect with the pad or not. The default setting is 25mil/side.

After defining the teardrop style and clearance checks as required, clicking OK will proceed to add teardrops to all selected pads. If placing a teardrop would result in violation of one or more checks, a pad will not be teardropped.

Continue selecting further pads to be teardropped, or press Esc to exit.

In order to apply the clearance constraint options, you must have extracted the netlist for the current document, before using the teardropping command.
A pad will only be teardropped if it has at least one trace connecting to it.
When teardropping pads, the effect of the inflated bounding rectangle will only be seen for pads that are grouped in a particular area. If pads are far apart in the design, the bounding rectangle used in the coarse teardropping check will be that of the union of individually selected pads, and therefore could extend to include the whole design, and slow down the process.
It is not advisable to teardrop pads in both your PCB Editing tool and the CAMtastic Editor. The results for trace/pad intersections would be less than desirable.

Trim Silkscreen

The Tools » Trim Silkscreen command from the main menus is used to trim silkscreen layer images, where they encroach upon solder mask layer pads.

After launching the command, the Trim Silkscreen dialog will appear. Use this dialog to specify a clearance constraint between silkscreen images and the edge of solder mask pads. Positive (retract silkscreen from pad) or negative (encroach upon pad) values may be entered.

Use the Copy to New Layer option to save a copy of the original silkscreen to a new layer. This can prove very useful when wishing to compare the results of the trimming operation.

After defining the trimming options as required, clicking OK will effect the trimming.

At least one silkscreen and one solder mask layer must be defined in the current document before this command can be used. The respective layer type (Silk Top, Silk Bot, Mask Top, Mask Bot) must be assigned to the appropriate layers in the Layers Table dialog (Tables » Layers).
When using the Copy to New Layer option, a layer, <designname>-old_n, will be created for each silkscreen-solder mask pair (e.g. one for top and one for bottom, if the layers exist and have been defined in the Layers Table dialog).
It is advisable to have just the solder mask/silkscreen layers turned ON when using this command. Not only does it make it easier to see which pads are being encroached by the silkscreen, it also allows you to compare original and trimmed silk layers without the clutter of other layers.

Create & Group Parts

The Tools » Parts » Create & Group Parts command from the main menus is used to create and group identical parts in the current design image, ultimately allowing you to generate a parts list that can subsequently be exported.

First, ensure that only a single top or bottom layer (e.g. Top or Bottom Solder Mask layer) is visible in the main design window, with all other layers turned OFF.

After launching the command, the cursor will change to a small square and you will be prompted to select a footprint. The procedure involves the following sequence of actions:

Use the cursor to select all pads in a particular footprint, either by clicking on each pad individually, or by dragging a selection box around them.
Right-click - the Assign/Group Parts dialog appears. Use this dialog to give the footprint a description (e.g. DIP14), specify its rotation, and define its type (Thru Hole, or SMT).
After defining the properties of the footprint as required, click OK. The software will look on the same layer only for identical footprints, searching in terms of size, shape, and orientation. Each identical part will have a rectangle drawn around it, with a cross running through its center. These cross-filled rectangles are added to a new layer - Refdes_Top or Refdes_Bottom - depending on whether the layer you are using to create the parts is on the top or bottom. This layer is added to the Layers list in the CAMtastic panel.
Continue selecting and grouping further footprints, or right-click, or press Esc, to exit.

You cannot group parts that have already been grouped. Therefore, selecting a footprint that has been grouped, and giving it a new description, will result in no change. You can however add a footprint of the same type to the parts list, by selecting the footprint and giving it the same description.
The part information is listed in the Export Part Centroids dialog (File » Export » Part Centroids).

Assign Reference Designators

The Tools » Parts » Assign Ref Designators command from the main menus is used to assign reference designators to all parts that have been successfully created/grouped in the current design document.

After launching the command, the cursor will change to a small square and you will be prompted to select a part. Simply position the cursor over the center of the cross in a grouped part, and click. The Enter Value dialog will appear, from where you can enter the reference designator you wish to assign to the part. After entering the designator required and clicking OK, the designator will appear at the center of the cross for the part.

Continue assigning reference designators to other parts in the design, or right-click, or press Esc, to exit.

Reference designators may contain any alpha and/or numerical character. Underscores may be used, spaces and other characters may not. The designator must be lowercase only.
Placing alpha-numeric designators will allow you to use auto-incrementing. For example, entering u1 for the first designator will cause designator u2 to be automatically available when placing the second designator, and so on. This can be of great benefit when assigning designators to parts of the same component.
The reference designator information will be added to the parts list in the Export Part Centroids dialog (File » Export » Part Centroids).

Convert Flashed Pads to Homebase Pads

The Tools » SMT Stencil » Homebase Pad Conversion command from the main menus is used to convert a pair of flashed pads to a homebase pad. Homebase pads are used for improving the area of paste (per pad) deposited with an SMT stencil.

After launching the command, the cursor will change to a small square and you will enter conversion mode. The procedure involves the following sequence of actions:

Select the initial pair of flashed pads to be converted. Simply position the cursor above each pad in the pair and click.
Right-click to access the Flash - Homebase Conversion dialog. Use this dialog to:
- Define the homebase pad in terms of the direction and extent of beveling that is applied to each of the pads in the pair.
- Choose to have the resulting homebase pads drawn on the same layer, a new layer or any one of the existing layers in the current document.
- Various other conversion options are available from the dialog, including the ability to set a flash tolerance - when searching pad-pairs for a match with the initial selected pad-pair - and whether to keep old pads or delete them completely.
After defining the options as required, clicking OK will return you to the main design window and you will be prompted to select the entire area to be considered for conversion. Simply drag a selection box around the whole design and then right click once the area has become selected. The selected objects will be compared against the initial selected pad-pair and all matches found will be converted to homebase pads.
Continue converting further flashed pad-pairs to homebase pads, or right-click, or press Esc, to exit.

The initial pair of flashed pads can be dissimilar in shape and/or size. The smaller of the two will be used in calculating the size of the homebase pad.
After conversion, each homebase pad is treated as a single object.

Add Epoxy Bars

The Tools » SMT Stencil » Add Epoxy Bars command from the main menus is used to add an epoxy bar between all occurrences of a selected flashed pad-pair combination, in the current document.

After launching the command, the cursor will change to a small square and you will enter epoxy bar addition mode. The procedure involves the following sequence of actions:

Select an initial pair of flashed pads. Simply position the cursor above each pad in this initial pair and click.
Right-click to access the Add Epoxy Bars dialog. Use this dialog to:
- Define the width and height of the epoxy bar, in relation to its position between the two pads.
- Choose to have the resulting epoxy bars drawn on the same layer, a new layer or any one of the existing layers in the current document.
- Various other conversion options are available from the dialog, including the ability to set a flash tolerance - when searching pad-pairs for a match with the initial selected pad-pair - and whether to keep old pads, or delete them completely.
After defining the options as required, clicking OK will return you to the main design window and you will be prompted to select the entire area to be considered for conversion. Simply drag a selection box around the whole design and then right-click once the area has become selected. The selected objects will be compared against the initial selected pad-pair, and all matches found will have an epoxy bar placed between them.
Continue adding epoxy bars, or right-click, or press Esc, to exit.

The Gap Factor of the epoxy bar indicates the width and height of the bar between the two pads. The width is a function of the horizontal distance between the pads (measured from the inside edge in each case). The height is a function of the vertical distance covered by the pads (measured from the top edge of the higher pad, to the bottom edge of the lower pad). Only values between 10 and 100 percent may be entered for these fields.
If this command is used twice in a single design session, the Add Epoxy Bars dialog will only appear if the initial pad-pair is different to that selected the first time the command was run. Otherwise, it is assumed that you wish to apply the same settings, and you will be prompted to select the conversion area directly.

Creating and Using a Macro

To record a new macro for actions carried out in the current document, choose the Macro » Start Recording command from the main menus. After launching the command, the Create New Macro File dialog will appear. Use this dialog to define where and under what name, the new macro script file should be stored. After clicking Open, you will enter recording mode. Any actions you carry out within the CAMtastic Editor will be recorded, and the corresponding lines of script added to the macro file (*.bas).

When you have finished performing all actions to be included in the macro, use the Macro » Stop Recording command to exit recording mode. The current macro recording session will be terminated and the generated macro script file will be opened automatically as the active document in the main design window. The generated file will appear in the Projects panel as a free document. The scripting language used is Enable Basic.

To edit a generated macro script, use the Macro » Edit Script command. After launching the command, the Open Macro File dialog will appear. Use this dialog to locate and open the macro file (*.bas) that you wish to edit. The macro file will open as the active document in the main design window. You can then edit the script as required.

To run the specified macro script, choose the Macro » Run Script command from the main menus. After launching the command, the Open Macro File dialog will appear. Use this dialog to locate the macro file (*.bas) that you wish to run. After clicking Open, the macro will be run, and the commands contained therein will be executed.

Версия для печати

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

Примечание

Набор доступных функций зависит от вашего уровня доступа к продуктам Altium. Ознакомьтесь с функциями, включенными в различные уровни Подписки на ПО Altium, и функциональными возможностями приложений, предоставляемых платформой Altium 365.

Если вы не видите в своем ПО функцию, описанную здесь, свяжитесь с отделом продаж Altium, чтобы узнать больше.