Greater control with the sketch in IRONCAD

LAST CHECKED:

October 29, 2026

Greater control with the sketch in IRONCAD
Emil Rindell

Emil Rindell

Jonas Bryntesson

Jonas Bryntesson

Henrik Andersson

Henrik Andersson

PUBLISHED:

2024-04-25

Emil Rindell

Emil Rindell

Jonas Bryntesson

Jonas Bryntesson

Henrik Andersson

Henrik Andersson

2024-04-25

The principles behind the Sketch in IRONCAD

Something else unique about IRONCAD is the principle with which you work in the sketch. That is, the plane, sometimes also called the "grid" or "Cross-Section", where you draw the lines that are the basis for different shapes such as an Extrude, which is one of four so-called Shape Features. But the sketch is also used by some Modification features such as Rib and Emboss etc.

The sketch in IRONCAD does not require "fully defined rules" through constraints to give you full control and precision, because there are several unique tools and some basic rules and features that we will take a closer look at in this blog post.

The sketch shows an aluminum profile, at the top without and at the bottom with blue endpoints and indicators.

As you have surely heard or read about before, there are many different ways to work in IRONCAD and some choose (actually!) never to learn how to use the sketch. "You don't really need to!". For those who think that it works well enough to quickly use "ready-made" 3D models from catalogs and easily manage them with handles - any thought of having to use the sketch can make them shudder!

For more experienced users, the sketch can be a necessity depending on how the model looks and needs to be modified, but it is not always so easy to grasp how it really works in a way that feels "fluid". However, it is quite striking how easy-to-use the tools you need to use actually are if you give them a chance.

To create a solid form via, for example, an Extrude Shape feature, only a number of lines that together form a closed contour are required. This can then be modified in a variety of ways, which may suit better or worse depending on when and where you are in the process, and of course which tools you know and master.

With handles, you can easily modify the lines in the sketch!

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Overview and contents

  1. Primarily, the sketch manages points, not lines.
  2. The selection acts as a temporary constraint.
  3. Extending lines, what happens then to the "connected" lines?
  4. Moving lines, what happens then to the "connected" lines?
  5. SmartCursor function
  6. Modify the sketch's lines directly via the Shape handles.
  7. Manage lines with blue "unlocked" Smart Dimensions (Reference Dimensions).
  8. Dark blue "indicators" show how a line will behave.
  9. Useful constraints to combine with "unlocked" lines.
  10. Tools with constraint options
  11. Better control of circular arcs and splines.
  12. The color says it all!
  13. Parametric table control of lines.
  14. How best to handle different types of "problems" when they arise.

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Before we begin - the sketch as a (2D) CAD tool...

‍If you are an experienced 2D CAD (read: AutoCAD) user, several fundamental steps, commands, and tools differ from how they are used there. This naturally means that you may experience certain steps as counterintuitive or unclear. That often happens when switching between different CAD/CAM systems. But keep in mind that the sketch is the foundation for 3D geometry and with IRONCAD you should spend as little time as possible having to use the sketch to change the shape and location of the lines that are there.

...and the sketch in comparison with other 3D CAD systems.‍

If you have been using another 3D CAD system based on the well-known and widely used Parametric Feature based principle, you are usually used to spending a lot of your time in the (2D) sketch and also usually "defining" it with various rules and limitations, also called constraints. In some cases, you cannot proceed without "fully defining" the sketch - > so that it is not possible to change its shape in any way with "some kind of unknown and uncontrolled freedom".

These types of rules primarily do not need to be applied in IRONCAD, mainly because there is no "unknown or uncontrolled form of freedom" of the kind you might be used to from other CAD systems. Instead, it is usually preferred to avoid constraints completely, but you can still have full control in almost all ways to modify the lines that are there. Something that for many at first may seem extremely strange or sound completely unrealistic.

However, this is possible because IRONCAD has a number of unique smart tools and flexible commands tied directly to the 3D models; for example, you usually prefer to modify the lines through handles instead of "going back" and editing the sketch. It is of course possible to use constraints and "fully defined" sketches even in IRONCAD, but you usually only do so when it is actually needed and makes a clear difference.

1) Primarily, the sketch manages points, not lines.

All the steps described below essentially handle "a point in an XY coordinate system". Every action performed will add or move one or more points in the XY plane, which leads to lines being created, changing shape, or moving. If you know that this is the foundation of the sketch in IRONCAD, you may more easily see and understand the principle behind the tools and the options available to choose from.

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Sketch 1a -Two Point Lines

A simple overview of the Two Point Line command, which is placed between two points (XY coordinates) in the sketch in ironcad. Keep in mind the difference between the right and left mouse buttons, where the right button (always) provides more options.

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Sketch 1b - Polyline

A simple overview of the Polyline command, which is placed between two points (XY coordinates) in the sketch in ironcad, but where you can continue with another line directly after the previous one. You can also easily switch to a circular arc. Keep in mind the difference between the right and left mouse buttons, where the right button (always) provides more options. Finish a line with a double-click of the left mouse button or end the command with [Esc].

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Sketch 1c - Rectangle

A simple overview of the Rectangle command, which is placed between two points (XY coordinates) between two corners in the sketch in IRONCAD. Keep in mind the difference between the right and left mouse buttons, where the right button (always) provides more options.

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Sketch 1d - Circle

A simple overview of the Circle command, which is placed between two points (XY coordinates) for the center point and radius in the sketch in IRONCAD. Keep in mind the difference between the right and left mouse buttons, where the right button (always) provides more options.

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Sketch 1e - End Points in the Sketch

The sketch consists of lines controlled by the end points where each line begins and ends. You work with points in an XY coordinate system that control the length and position of the lines. The end points can be moved "freely" by dragging them with the mouse cursor, or with various types of "control" based on what you have selected.

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2) The Selection acts as a temporary constraint

By selecting one or more lines, you temporarily constraint what can and cannot be changed. This is a big difference compared to placing permanent constraints! A selected line will follow other lines that change shape.

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Sketch 2 - Selection, an important control in Sketch

Selecting objects in the sketch is a simple but important way to gain more control. Selected lines will move when another line changes length. Keep in mind that it is always the endpoints of the lines that move when you move or change the length of the lines!

3) Extending lines, what happens to the "connected" lines?‍

When a line is extended, the connecting line will be affected and thus forced to change its shape or move. But how can you predict what will happen before making the change and without using constraints? Remember that it is always the lines' end points that move when you move or change the length of the lines!



Sketch 3a - Selection controls change of direction in the Sketch

Depending on which side of a line you select, you control the length in that particular direction. Remember that it is always the end points of the lines that are moved when you move or change the length of the lines!

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Sketch 3b - Changing line lengths and managing Maintain End Conditions‍

When a line changes length (the end point moves), you can control how connecting lines are affected—whether they should move along and maintain their angles or change their length and angle. This is controlled via the Maintain End Conditions setting. This property is only displayed when editing the "selection dimension" (Curve Dimension) on a line and is (unfortunately still) not possible to control via the Property Browser, where this property is always "off".

Without knowing this, it is easy to feel that the sketch lacks precision and control.

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Sketch 3c - More control over length and angle with the Curve Dimension handles‍

When a line or circle is selected, a dimension is displayed by default through the Curve Dimension function, allowing you to change length, angle, and radius. This function also features smart handles so you don't need to know the exact dimensions you are aiming for. Just like with the handles on Shape features, you can drag and snap to other geometries!

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4) Moving lines, what happens to the "connected" lines?‍

When one or more lines are moved, the connecting line(s) will be affected and thus forced to change shape or move (the end points move). How can you predict what will happen before making the change and without using constraints? Depending on which commands are used or if you combine them with various keyboard shortcuts, you can gain full control over this. The SmartSnap function is also available here, displayed as a green point to help you find other geometries to snap to.

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‍Sketch 4a - The Move command on lines connected to other lines

When using the Move command, it is good to know how connecting lines behave depending on whether they are selected or not. This is particularly true for lines that are not connected at a right angle but at an oblique angle. Remember that it is always the lines' end points that move when you move or change the length of the lines!

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‍Sketch 4b - Moving lines and using SmartSnap

When you select and drag a line with the left mouse button, the nearest end point will utilize the SmartSnap function, which appears as a green point and indicates where the dragged line will end up—for example, the "closest corner" of a simple rectangle. You can also use this to find intersection points between angled lines and 3D geometries.

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‍Sketch4c - Unlock temporary relations with [Shift].

When drawing a line, you can temporarily unlock temporary relations with other lines by holding down the [Shift] key while moving the line with the mouse pointer. The precision then lies in the fact that SmartSnap can snap to the end point closest to the mouse pointer where the line is drawn. The connected lines must adapt their length and angle to solve this. This is also shown in point 10b Chamfer.

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Sketch 4d - Temporarily lock along XY coordinates with [Alt]

When dragging an end point or lines, you can hold down the [Alt] key to lock against the XY axes.

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5) SmartCursor function.

IronCAD was early to develop a feature for the sketch called SmartCursor, which means that the mouse pointer and the selected object work together to find interesting information in its vicinity. This is shown by green dashed lines appearing around the cursor, e.g. when dragging an endpoint or a line.

The SmartCursor displays green dashed lines as assistance from other lines.

If there is too much information, you can temporarily turn off the SmartCursor function by holding down [Shift]. However, you still retain the ability to use the SmartSnap function to snap to other lines or the sketch grid. SmartSnap is displayed as a green point near the mouse cursor.

SmartSnap with its green point next to the mouse cursor. SmartCursor is temporarily turned off via the [Shift] key.

If you do not want to use SmartCursor at all, you can permanently disable the function under the Snap settings. Then, green dashed guide lines will no longer be displayed in the sketch.

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6) Modify the lines of the sketch directly via the Shape handles.

Something that IRONCAD has done very well since its inception is to allow the user to modify the lines in a sketch through visual easy-to-use handles that appear in the "regular 3D modeling mode". These handles are called Shape handles and usually appear at the corresponding mid point of each line, but only when the mouse pointer is near that particular line. For circles, the handles appear on a quadrant and control the radius of the circle, but you cannot move a circle using any handle.

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Sketch 6a - Use the Shape handles to modify the lines in the sketch

Instead of "going back" to the sketch to make changes such as moving lines, you can use the smart and easy-to-use Shape handles displayed on each line.

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Sketch 6b - Associate a Shape handle with a geometric edge

On the right-click menu of a Shape handle is the Associate to Edge option. This creates a permanent lock through a Project Constraint in the sketch. You can no longer access the menu for the handle, as the edge/line is now associated to another edge. By editing the sketch, you can reach the constraint and remove it, if you want.

NOTE! Keep in mind that you cannot visually see this association/constraint once it has been applied, even though it is there. The constraint is only visible in the sketch.

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7) Check lines with blue "unlocked" Smart Dimensions(Reference Dimensions)

Instead of using red and locked dimensions (Smart Dimensions) that do not allow you to change the length or position of lines in any other way, you can unlock them -> but they still retain an interesting feature. They then act instead as a unique combination of "reading and driving dimensions" (these are also referred to as Reference Dimensions) and you can directly see the length of a line or the distance between lines.

These dimensions are shown in a dark blue color instead of the red (locked) color. It is still possible to change a dark blue dimension and if you double click on one of the dimension arrows you can control the direction of the change.

To "unlock" a red Smart Dimension, right-click and uncheck Lock in the menu. The color will turn blue and the dimension text will update in real time if the point or line is moved with the mouse cursor or a Shape handle.

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Sketch 7 - Unlocked (blue) Smart Dimensions

Here is an example combining the freedom of Shape handles with lines managed via red locked Smart Dimensions (Constraint Dimensions) or blue unlocked Smart Dimensions (Reference Dimensions), and why this is a useful and smooth combination.

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8) Dark blue "indicators" show how a line will behave.

There is a feature in the sketch called Profile Condition Indicators, small blue symbols that can appear next to certain lines to show their "temporary relationship" to the sketch's XY coordinate system or to other lines.

This is not a constraint-based lock, but rather primarily "an indicator of how the line is currently oriented within the sketch or relative to other lines". However, you can easily lock such an indicator into a constraint by double-clicking it or via the right-click menu on the indicator itself.

These blue indicators are displayed "centered" along lines that are "parallel to the XY coordinate system" as well as "at the corners" between lines that have a "perpendicular relationship" to each other.

They can also appear as blue dashed lines with an indicator showing the temporary relationship between lines that are not directly connected to one another. Hovering the mouse over an indicator highlights in orange which lines are indicated to have a temporary (blue indicator) or permanent (red indicator) relationship with each other.

They also appear between lines, circles or arcs that have "smooth" tangent relation. When locked as a constraint, they are shown in red, which we'll look at later. By placing the mouse cursor on an indicator, an orange color shows which lines are indicated to have a temporary (blue indicator) or permanent (red indicator) relationship with each other.

Under the sketch's Snap settings (right-click in the background), you can control which types of indicators should be displayed in the sketch.

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9) Useful constraints to combine with "unlocked" lines.

Although it is generally not recommended to use constraints in the sketch in ironcad unless you are entirely sure you need them or want to parameterize lines in the sketch, there are certain situations where a few types of constraints can be useful and provide a bit more control under specific conditions.

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Sketch 9a - Tangent constraint

It can be difficult to "freely" draw endpoints and lines when there are arcs connected. Without a "smooth" tangent transition you get an ugly "crease". This Tangent relation is shown by an indicator that can also be locked as a constraint.

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Sketch 9b - Horizontal and Vertical constraint

By locking a line parallel to the X or Y coordinates, you ensure that the lines can only follow parallel to the coordinate system. This avoids unwanted angles on "straight lines". However, it can also complicate things, as it prevents you from angling a line, which can cause other lines to "shoot off" over a long distance.

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Sketch 9c - Project constraint

Projecting contours from other 3D models while creating a locked relationship with the geometry. If the other geometry changes shape, it will immediately change the shape of the projected lines in the sketch.

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10 - Tools with constraint options

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Sketch 10a - Fillet with and without constraints

With the Fillet command, you add radii as a kind of feature, with or without constraints, between lines. Keep in mind the difference between the right and left mouse buttons.

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Sketch 10b - Chamfers with and without Constraints

If you need a chamfer between two lines, you can use the Chamfer command. It has several measure-driven variants where you can also choose to add locked dimensions as constraints. This video goes through the different variants and compares the difference between them. Keep in mind that it is usually an advantage to add a chamfer as a Modification feature, so you can more easily reach it to change or suppress. Having simpler shapes in the sketch also makes the handles easier to use and gives more predictable results.

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Sketch 10c - Mirror with constraint

When mirroring lines in the sketch with the Mirror command, you can choose to simultaneously create a constrained relation between the lines that are mirrored. However, there is no difference between the lines in terms of"Master/Slave", which makes it easy to change whichever side of the lines you need to change.

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Sketch 10d - Offset with constraints

With the Offset command, you can apply a locked dimension that controls the copied lines, which can also be accessed outside the sketch.

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11) Better control of circular arcs and splines.​

We have created a video demonstrating how to control all dimensions of a long, rounded connecting rod. This is a shape that cannot otherwise be adjusted in a predictable manner using handles or any form of "freedom" in the sketch. Here, locked dimensions and relationships provide a fully predictable model.

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Splines can be controlled using the insertion points located along the spline curve. Each point can be driven by dimensions.

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12) The color says it all!

The lines in the sketch can be displayed in several different colors but the most common color of lines is black (formerly white). However, it is good to know when and why certain lines are sometimes shown in a different color!


Under Defined -> Black

Black (formerly white) thick lines are called Under Defined and represent the default mode in the sketch in IRONCAD. Since they are not managed by locked relations and constraints, you can make very many types of changes with them, sometimes even "illogical" -> remember that it is the endpoints that govern and the lines on each side of the endpoint must adapt accordingly! This is also the reason why they are handled as Under Defined by the system, they lack "enough" constraints to be handled e.g. by a parameter table and can therefore easily be changed by handles "outside" the sketch.

Keep in mind that Under Defined never means "out of control" in IRONCAD.

This is a fantastic strength and flexibility that opens up with IRONCAD and something that is definitely very useful to learn; there is still no equivalent way to modify lines in a sketch with any other 3D CAD system on the market today.

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‍Fully Defined -> Green‍

Green thick lines mean that the lines are "fully defined" and can only be changed in the ways specified, with visible and locked dimensions and relations between lines and the coordinate system. It is no longer possible to change the length or position of a line "freely" with the mouse pointer or via smart handles. However, this is a purely "mathematical definition" where all the relations and rules (constraints) required for length and position to be controlled from, for example, the parameter table or by other lines have been set.

NOTE! This does not mean that you have better precision or necessarily more control, which one might otherwise think.

With constraints in IRONCAD you move from the freedom to change "with full control and almost infinite possibilities" (which requires more knowledge of how to do it) to only being able to change "in a predetermined and fully defined way" (as a kind of "programmer of geometry"). Sometimes this works very well, e.g. with table-driven standard components. But in normal machine design or in a large layout it can be devastatingly slow and some changes are impossible to make, you often have to start from scratch as the rules and relationships you have defined at an early stage are no longer valid.

Keep in mind that you can combine this "freedom" with constraints in IRONCAD in a unique way that suits you or the model you currently need to develop!

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OverDefined-> Red‍

Red thick lines mean that there are "too many" constraints that contradict each other, and you will likely need to remove or unlock one of the constraints that conflicts with another.

NOTE! Keep in mind that you can use "blue dimensions" that are "unlocked". You can still see the dimension and even change it, but it is not a locked dimension that can be controlled by other dimensions or from the parameter table.

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Lines in relation to each other -> Orange

If the mouse cursor is placed on a blue indicator or red constraint, an orange color appears on the lines that together have the relation that the indicator or constraint corresponds to.

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‍Construction lines -> Dark blue‍

Dark blue thin lines mean that the line is of the construction geometry type (Construction Geometry) and that it will not create any 3D geometry from these lines in a sketch that subsequently builds a Shape feature of some kind. It is most often used as a reference (construction line) to work against and can also be a convenient alternative to deleting them completely. You can compare it to "hiding" (suppressing) lines instead of deleting them.

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Highlighted lines -> Yellow

Yellow lines mean they have been selected by the mouse pointer and will be affected by the running command, or that they are statically moved in the sketch if multiple lines are selected in yellow.

This is also a form of "light constraints" that are only used "temporarily in the moment" and then released as soon as the line is deselected with a simple left click in the plane of the sketch or via [Esc]. Very fast, smooth and powerful, which makes it possible to avoid having to create constraints that are more permanent and that you always have to deal with.

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‍Failing lines -> Magenta/Pink‍

When you finish the work in the sketch and finish to create the 3D geometry, you may encounter different types of problems for various reasons. Intersecting lines or lines with red endpoints appear as thin lines with a magenta (pink) color.

Tip: If the pink color of the line does not return to the "correct color" - try drawing a new line and deleting it, or trimming a line and undoing. This usually updates the graphics and the color of the lines.

More on this further down under point 14) How to best handle different types of "problems" when they arise.

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Offset Spline -> Cyan blue

When using the Offset command on a Spline curve, the copy turns cyan blue.

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13) Parametric table control of lines.

‍If you choose to use parametric control of lines in the sketch, there is quite a bit to keep in mind. The lines should generally not be movable or draggable "freely" with the mouse pointer, and some, many, or all lines are controlled by other geometries or via numbers and rules in the parameter table.

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Fully Defined Sketch

When all lines in a Sketch are completely "controlled" by constraints and fixed dimensions, the Sketch is called "fully defined". All lines then have a green color and you can no longer "freely" drag endpoints or lines with the mouse cursor. The shape handles also completely lose their function and you might as well turn off the display of these via Shape Properties.

Depending on the shape of the geometry, a fully defined sketch may be a requirement to parameter-drive a profile in a completely predictable way (regardless of the CAD system).

As we can see in the image, certain criteria must be met. Here are some common requirements;

  • All line types' endpoints and/or lines must be controlled in position and/or length/angle with locked dimensions.
  • All circles must be controlled in position (center) and radius/diameter with locked dimensions.
  • All fillet radii must be controlled with locked dimensions.

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Sketch 13 - Parameter table with the Sketch in IRONCAD

In this video, a parameter-driven fully defined rectangle is controlled via Edit Cross-section (the sketch) on a block, where the lower left corner of the rectangle is locked to the origin. The vertical and horizontal lines are locked and dimension-driven. These dimensions can then be linked and controlled via the parameter table.

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If you are interested in learning more about how to parameter-drive models in ironcad, you can read more about it in a separate support blog post.

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14) How to best handle different types of "problems" when they arise.

First ofall - it is not possible to finish a sketch building a Shape -feature if any of these three "problems" have occurred in the sketch. If this happens and you see this message, choose either Edit Cross-Section (green highlight) or Create Default Shape (yellow highlight).

Avoid clicking Cancel or the close button (red highlights), as these options revert back to before you started editing the sketch!

If you encounter errors in the sketch, avoid the red-highlighted options.
  • Edit Cross-Section - Go back to the sketch and "fix" the error.
  • Create Default Shape - The error is ignored and a large 3D block is created. You can save the 3D scene and can edit the sketch at a later time.
  • Cancel Edit / Close the sketch window - Cancel and start again. NOTE! Everything you have drawn will disappear. This cannot be undone.

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Empty sketch

This one is perhaps obvious. It is not possible to execute a sketch that is empty.

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Crossing lines

Lines that cross each other will appear in pink/magenta color when trying to finish the Sketch and need to be trimmed or removed.

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‍Duplicate lines‍

A kind of variant of crossing lines are lines that "lie on top of each other as duplicates" in the sketch. However, upon import, all duplicates will be automatically deleted.

Use the Clear Duplicate command to search for and remove these.

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Red end point / "open" profile

A sketch building a Shapefeature cannot be finished if there are endpoints of two or more lines that are not connected to each other. The lines ending in a red endpoint will appear as pink/magenta lines when trying to execute the sketch.

With the Find Gap command, you can find "gaps" between red endpoints within a range of the dimension you set. It does not have to be a "gap" between lines, but can be a simple line with each end marked in red.

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‍Zero length line‍

You can accidentally click out "an extra point" at the end of a line, resulting in a "zero length line". This "zero-length line" is very poorly visible but actually appears as a "slightly larger endpoint" behind a "regular endpoint". By box checking around the endpoint and then pressing [Delete], the point disappears and you can finish the sketch.

When importing a DWG or DXF file, these "zero" lines should automatically be sorted out and disappear.

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