LAST CHECKED:
October 29, 2026


Emil Rindell

Jonas Bryntesson

Henrik Andersson
PUBLISHED:
2022-03-09

Emil Rindell

Jonas Bryntesson

Henrik Andersson
2022-03-09
There are numerous settings in IRONCAD managed via IRONCAD Options. On this page, we review the most common settings that we recommend checking. Most of these settings are configured automatically during the installation of our Swedish Standard Customization, but you can of course use this guide to adapt and adjust them to suit your specific needs!
You can quickly find IRONCAD Options via this icon in the Quick Access Toolbar at the top of the software.

Using the Load and Export buttons in the bottom-left corner of the Options window, you can save and open your configured settings. This makes it easy to restore settings or apply them to another computer.

You can use the Search Options button to search across all available settings under Options.



Show Welcome dialog on startup
Display the Welcome dialog (for creating new files or opening existing ones) upon startup.
Show Welcome dialog when no documents open
Display the Welcome dialog when all open files are closed.
Number of recent files want to show
Set the number of recently worked-on files to display in the Welcome dialog list and the application menu.

Show warning of file link reference changed due to SaveAs
A warning is displayed when you rename a 3D file and it is linked upwards to something that uses it, such as a master file or a 2D drawing. That file ("above") will then use the new file that you saved. NOTE! This only applies if the main assembly or 2D drawing is open at the same time, so that the link between the files is active. Otherwise, the link will not change. So be sure to close all linked files before saving a copy of a sub-set or part, unless you want to re-link them to a new file at the same time.
Show warning when linked shape names are inconsistent
A warning box will appear when the file is opened if any internally or externally linked smst or part has different names in the tree, even though they are set to use the same name. This can be caused, for example, by working with an externally linked part and later opening the smst containing it and more links of it. The usual practice is to use the linked "User Name" for this instance. The second option Keep the current "User Name" and set the properties to "Only this part" means that you will be able to use a unique name for linked smst and parts.
NOTE: Ensure you do not save this setting if the warning appears when opening a file, as it will become a permanent setting that must be manually changed here afterwards.

Precision displayed in dialogs
The number of decimal places in dialog boxes; reduce to 2 or 1 if necessary. However, it is often advantageous to view more decimal places in dialog boxes than directly in the graphics area (below).

Dimension precision
The number of decimals directly in the 3D graphics; feel free to reduce to 2 or 1 depending on how many decimals you want to see.
Please note that the number of decimals displayed in dialog boxes may be rounded. IRONCAD uses the Parasolid and ACIS solid kernels, both of which are based on 10-6 meters (which is 0.001 mm). You don't see all the decimals all the time, but they are there. What you can then physically manufacture "in the real world", depending on the manufacturing method, affects how accurately you need to show the dimensions in a drawing. But all measurements are always based on 10-6 meters.

Dimension Font Size
Controls the size of dimensions and other text in the 3D scene; consider increasing from 15 to 20 or 22 (appearance varies depending on your screen resolution).
Number of undo steps
The number of undo steps; 20 is now standard and you don't really need to set much more. Work in the Sketch (cross section) is usually where you use multiple steam steps most of the time. Otherwise you can easily adjust changes that got wrong with TriBall or handles directly, instead of undoing.

Enable file save reminder
With this setting enabled, you receive a reminder to save the file at X min intervals, which is set numerically in the box next to it.
Track open file modified by others
If multiple people are working with shared files (external links) and making changes, you can receive a notification that a specific incoming file has been modified by someone else. The file must then be manually closed and reopened to load these changes. Set the desired check interval in seconds.

Enable camera Look At during editing
With this setting active, the camera view automatically rotates toward the grid when editing the cross-section (Sketch). Turn this off if you do not want an automatic camera rotation when selecting Edit Cross-section. The setting below resets the camera settings once you are finished in the cross-section.
Enable camera Parallel during editing
With this setting active, the camera's perspective function is turned off when editing the cross-section (Sketch), which is recommended. The setting below resets the camera settings once you are finished in the cross-section.


Default kernel type for new parts
The basic setup is Parasolid, which is the most common solid kernel in 3D CAD and 3D CAM. If you work a lot with e.g. AutoDesk Inventor, it may work better to change this basic setting in IRONCAD to ACIS when sending and receiving files in e.g. STEP format. However, most other 3D CAD and 3D CAM systems use Parasolid as their solid kernel.
TIPS. To quickly see the effect of changing the solid kernel on an existing Part: "Ctrl + K".

Part Regeneration
Checks how the recalculation of parts is done. The usual one is the automatic Regenerate the part automatically. But if you have more complex models with many features, you can change this setting to Wait to regenerate until the part is deselected. This means that the model will not be recalculated until it is deselected, no matter how many changes are made to different parts of the model. Not only does this make the program feel faster, it also makes working with complex models easier.

Surface Smoothness
Control the edge roughness of new parts created. Default is 30 and should generally be kept at this value. However, this value can be increased (e.g. to 64) if the graphic perceives edges of parts as choppy. However, keep in mind that higher edge roughness affects file size, regeneration times and also the 2D drawing may update slower at too high edge roughness of the parts. It does NOT affect the accuracy when exporting to e.g. STEP or Parasolid. This is only a representation setting that affects IRONCAD and how it handles circles etc. However, when exporting to 3D printers, you control this value and when exporting STL, the settings are shown in the export box itself.
Helix Smoothness
The corresponding setting for so-called "helix" shapes—such as screws or springs. Can advantageously be set down to 10 by default

Default Intellishape Reordering Setting
A patented IronCAD technology that allows features (Intellishapes) that make up parts to automatically change the order of rotation to take effect. Can be turned off, then select Disable Part Reordering. The disadvantage of disabling the feature is that the regeneration times of individual parts will be longer, as it reads the whole tree and not just the features affected by the change.

Ghost Part/Assembly
Consider enabling the ability to snap and drop models from catalogs onto "Ghost" objects; it is disabled by default but more convenient when activated.

Choose tree item display type
Control what should appear as the name of the assembly and parts in the story tree. Part Name (also called User Name) is the default but many are now starting to combine e.g. Part Number and Description to be able to directly see where and what you have filled in and where you have not done so.
When saving, construct the filename from
Controls what the software automatically suggests as a file name when saving a new file. The default is the name of the first model in the tree, Part Name (also called User Name). Many users also change this so that the file name is automatically adjusted to the current Part Number and Description used for the first item in the history tree (when saving the file) or for the item selected when exporting an external link or copy.


Keep Part/Assembly order when creating assembly or copying them
Disable this option because it works better when the order is controlled by how you selected the objects, not their previous order in the tree before selection. If you have worked with IRONCAD for many years, having this setting enabled might feel unusual at first.

When dropped on pattern or linked feature
Controls whether you automatically get linked copies of an item dropped from a catalog onto all identical shapes where it is dropped. For example, if you drop a screw onto a linked hole, all linked holes can have linked screws positioned.

Large Assembly Mode
It is recommended that you turn it off, as the function disables all possibilities to change the models. With our Swedish default customization, we have turned off this setting and at the same time adjusted up to 5000 parts (medium assembly). The setting gives better performance, but it also cuts off the possibilities to modify the file, much like working in a 3D Viewer.


Use snap as default handle behavior (without Shift key)
Determines whether to use the [Shift] key or not when snapping to other geometry. With this option enabled, you use the [Shift] key to avoid snapping to other geometry, which many users find counterintuitive.
Maintain geometry of adjacent curves when dragging profile curve
When dragging with Shape handles, you can control how connecting lines at an angle other than 90 degrees are handled. The default setting (active) reduces the length of the line being dragged, and extends and maintains the angle (see the right line) of the two connecting lines:

Disabled, maintains the length of the dragged line, forcing connecting lines to extend and potentially change their angle (see the line on the right):

Show edit toggle icon upon selection
Controls the display of the white button that switches the handle type between red round Sizebox handles or red square Shape handles. Note that the [TAB] key on the keyboard has the same function!

Automatically switch to next sizebox handle value after enter
Means that you automatically jump to the next handle when pressing [Enter]. Most users keep this function disabled.
Disable Symmetrical Handle Toggle
Disables the Symmetrical Handle Toggle button shown inside the handles, which locks them symmetrically over time. Tip! Right-drag the Sizebox handle for symmetry.
Disable Symmetrical... enabled:

Disable Symmetrical... disabled:

Enable Dynamic Sizebox Dimension Display
The dimension box (Sizebox Dimension) stays attached to the cursor instead of appearing in the middle between the handles. We have left this active, as many users have requested precisely this feature.
Enable Dynamic Sizebox… enabled:

Enable Dynamic Sizebox… disabled:


Automatically add position dimension on dropping feature
Automatically adds one or two SmartDimension measurements from the nearest edge(s) when dropping features from a catalog. The same principle applies to holes on Sheet Metal parts.

Default location type
Default setting for 2D Shape placement. Selecting Point from the drop-down menu means that with a single click you can directly position the drawing plane and then fine-tune the position with TriBall. Also set Continue as the default for how the camera will adjust when zoomed in so close that the grid does not fit on the screen. With Continue, the camera does not change position or zoom, but remains with parts of the grid outside the visible area on the screen.

Enable master shape positioning
Means that you can light the TriBall on the basic shape in a TriBall pattern. It is usually inactive by default but is perfectly ok to activate.
Reset TriBall to copy
Means that TriBall is automatically moved to the copy and can also be checked in the copy/link box itself.

Show TriBall Activator Icon
Control whether you want to see the blue TriBall icon displayed at the anchor point of each selected object in the 3D scene. The icon can also be right-clicked to temporarily hide it, e.g. if it is in the way of the round red Sizebox handles or the measure.

Default Focus for Copy/Link Dialog
Controls whether Count or Distance/Angle should be selected first. Many prefer Distance/Angle, as it is easy to accidentally type a large number, say 1000 pcs, instead of a distance of 1000 mm.


Intellishape from 2D Shape
What should happen when a 2D Shape is loaded as a feature in a part. Should it be Consume, Copy or Link.

Auto select dropped object
Retains the selection on the object dropped from a catalog.
Drop assembly/part into selected assembly
The object dropped into the 3D scene will automatically become part of the currently selected assembly.
Show design variation dialog when dropped object
Displays the dialog box for Design Variations (parameter-driven models created in ironcad).
Show dialog when dropping text property catalog items
This setting applies to the checkbox that appears when dragging a text property out from a catalog.

Show resize shape dialog
Displays the Resize Shape dialog box. This means if the new part is scaled to fit the camera view.



Show part name tooltip
Shows or hides the white label that appears at the mouse cursor when clicking objects in the 3D scene.

Orbit about cursor location
Means rotating around an object if the mouse cursor is positioned over it. Otherwise, it rotates around the center of the screen.

Finish command and dialog when click middle mouse button
Allows you to execute feature commands with a single click of the scroll wheel.

Zoom to cursor location
Means zooming in toward the mouse cursor's position on the screen. Turn it off to zoom straight in/out instead.
Reverse zoom direction
Reverses the zoom direction based on the scroll wheel; instead of zoom in, it becomes zoom out when rolling the wheel in a certain direction.

Mouse Gesture
Provides the ability to start and execute commands via mouse gestures (displayed as orange lines in the graphics area) when holding down BOTH the left and right mouse buttons simultaneously. Here you can disable this function if you happen to trigger it by mistake or do not wish to use it at all, as well as set the delay time (time for simultaneous left-and-right press) before the mouse gesture activates, and view information (popup mouse gesture list) about available mouse gestures.



Working directory
This is the folder suggested when saving and opening files right after launching the software. If you have started working with files in a specific project, this folder opens when you choose to open files. If you have saved files in another folder, the last folder you saved to is always displayed.
Template directory
The file path for 3D, 2D, and BOM templates in ironcad. This path can advantageously be placed on a shared file server if multiple users are working in ironcad and using shared 2D drawing templates.
Tip! Or place templates in Public Documents to avoid being restricted by IT policies or permission settings.
Default path for templates (from 2020 PU1 SP1):
C:\Users\*YOUR USER*\AppData\Roaming\IronCAD\IRONCAD\*22.0 AND LATER*\en-us\Template
In earlier versions, templates were located here:
C:\Program Files\IronCAD\*2020 AND EARLIER*\AppData\en-us\Template


Display Sheet Metal feature shape handle as default
Controls whether to use the red round Sizebox handles (when Off) or the red square feature handles (when On) by default. The difference is that you either stretch (scale) all lines simultaneously (Sizebox) or work with them individually (feature).
Display Sheet Metal unfolded direction arrow
Choose whether to have an arrow showing in which direction the sheet metal part is unfolded.

Set new unfolded Sheet Metal part as “Included in BOM”
Controls whether the unfolded sheet metal should also automatically use the Include in BOM setting and thus appear in the bill of materials on the 2D drawing. Combined with the bottom setting for copying Part Properties over to the unfolded sheet metal, these almost always belong together—either both are active or both are disabled.
Part Properties for flat are copied from folder part
Controls whether properties (Part Properties) from the checked plate should be copied over to the unfolded plate when it is created (when unfolded).
Set Keep Unfold Supressed State for new unfolded Sheet Metal part
When unfolding a sheet metal part, you can manually select certain other objects to be visible (not suppressed) for each object afterwards. When you then unfold again, IRONCAD has "forgotten" which parts that were not suppressed. But with this setting you can have the unfolded part to remember what is not suppressed. The setting avoids having to select it every time you unfold.

Display stock selection dialog on dropping stock
Displays the stock table when a new sheet metal stock is dropped into the scene.

Use Stock name as Material
The name of the stock is entered as a material under the material properties.

Use Stock Name as Description and Code as Material
The name of the sheet metal is entered into the Description (under Part Properties) and the material code into the Material properties.

Auto-Maintain bend alignment for newly created bend
This setting controls how the First Bend Stock is handled when the bend angle changes. It is similar to the settings for Second Bend Stock.
With this setting turned off (not recommended), the length value of the First Bend Stock will change when the angle changes to maintain the total amount of material (even though the angle changes). This means material is added between the bend and the connecting stock when you change the bend angle. If you enable this setting instead, it becomes more predictable in that no extra material is added between the bend and the next stock when changing the bend angle. Usually, you want the First Bend Stock Length set to 0 min, just like with the Second Bend Stock Length. This means the bend sits flush against the edge it was dropped onto, with no extra material squeezed in between.
Bend line angle in drawing measured down from 180 degrees
Some press brakes count down from 180° instead of up from 0°. With this setting, the bend information transferred to the 2D drawing is updated accordingly. For example, 45° becomes 135° instead.
Align bend end on Drop for In our Out Bend
New in v2020, the ends of In Bends and Out Bends automatically adjust so you don't have to drag the feature handles (or enter numbers under Bend Properties, Corner Reliefs) to change from a flat end to a smooth transition at the ends:
With the feature set to Active, notice how the ends are not "flat" (default setting from 2020):

Disabled (as it was before v2020), most clearly visible on the right end (Left according to reliefs):


Bend Reliefs
Controls the standard shape and dimensions for the relief cuts at the ends of bends, which can also be accessed individually via the red square relief handles on a bend.


Second Bend Stock Length
At each end of a bend, there is an option to extend it straight out from the end of the bend, which we refer to here as the "bend length extension". The length extension located on the opposite side to the flange where the bend is attached is called Second Bend Stock. There are four different options for how this length extension is calculated when the bend angle changes: Flange, Tangent, Inner Sharp, and Outer Sharp. There are also three options under Update Behavior that control how, or if this length extension should change at all when the bend angle is modified: Default, Maintain unfolded length when changing angle, and Maintain specified length.

Create punch and forming constraints
Automatically inserts 2 dimensions relative to the nearest edges where the hole/punch form was dropped; applies only to shapes from the SheetMtl catalog.
Display constraint dialog after drop of punch and forming shapes
Displays a dialog box where you can enter dimensions and choose to constrain the shape to the edges of the sheet metal. These settings can be accessed at any time via the right-click menus of the dimensions.
Auto-Constraint bends
Automatically creates a constraint for each bend relative to the edge where the bend is dropped. When edges are moved, the bend follows, but it is never extended (shape-modified).
Auto-Associate to attached entity
Instead of creating a constraint property, each new feature created when dropped from the SheetMtl catalog onto a sheet metal edge is associated with that edge. The advantage of this setting is that bends and sheet metal parts are automatically extended when the edge they are attached to is extended. This saves a lot of time!
See more here: https://www.youtube.com/watch?v=GlyWx6Kl_SE&feature=youtu.be

Advanced Options

The Advanced Options... button controls the settings for the size of a new sheet (Stock) when it is dropped into the 3D scene, as well as the default setting for Bend corner treatment, which governs the default gap size between parts in the sheet metal, for example when using the Snap to point for corner option on a relief handle.
New part size – controls the standard size for new sheet metal parts created by dragging and dropping them from the catalog into the scene.
Bend allowance - checks whether it is the sheet metal table, per individual stock, or the standard DIN 6935, generally for all sheet metal, that should be used to calculate the compensation for cold-bent sheet metal in IRONCAD.
Punch Positioning Mode – controls how a Punch/Tooling feature (blue and green icons in the catalog) is positioned when dropped so that it is affected by a bend. Active = In relation to the unfolded sheet metal (recommended). Off = Positioned directly on the bend (not in the flat pattern), most likely without displaying any dimension from an edge, making repositioning more difficult (not recommended).
Bend corner treatment – controls the default setting for the gap that occurs when using the snap function Snap to Point for Corner on a shape handle.

Here you can select the standard thickness for your sheet metal from a list. The sheet metal type highlighted in the list is used when you drag a new sheet (Stock) into the 3D scene. The active sheet metal type is displayed at the top. Below the list are two path settings for the file listing all sheet metal thicknesses and tools, such as a network path to a file that multiple users can share.
OBS! If you have downloaded either of the two settings files at the top, you need to check the paths to the sheet metal tables.


Full Multi-Threading (needed for Point Cloud)
If you work with point clouds, it is important to enable this setting. For certain add-in functions such as DDM, it is important NOT to have this function active.

Driver type (Graphics engine)
IRONCAD offers various options that may suit different graphics cards. If you experience graphics issues, try changing the graphics engine from OpenGL to DirectX. This can make a big difference for lower-performance graphics cards.
(NOTE: Close all open documents first).
Display List
Segment is generally said to work best, but it depends on your computer, so you should test the three alternatives: Auto, Segment, or Geometry.


Compute mass for part and assembly automatically
This setting affects the regeneration used to calculate the mass (weight) of parts and assemblies. Recommended to be turned off to save performance.
Auto preview when edit feature
When this is active, a preview is displayed directly when editing a feature, such as a Blend. To save performance, it is recommended to keep this turned off.
Do model check after feature command
Runs a check on the created feature. Recommended to be turned off to save performance.
Load the exact surface description (brep) when open file
In order to save performance and, above all, time, when opening files, not all the information is loaded immediately when the file is opened. This results in a grey border color on parts that are not fully loaded. As soon as a feature is selected, the entire part is regenerated and then given a cyan blue border colour.

Use Cached Graphical Display Data
This setting is intended to speed up the time it takes to open files. However, you can disable the function if you experience graphical issues, as the file's saved graphics data (cache) is automatically reset as soon as the file is opened.
Use Visual Load when Opening Files
Uses a function that opens the graphical part of an ICS file in a fraction of the time required to open the entire file. While this is happening, no tools other than the camera (zoom and rotate) can be used.
Hide small parts automatically
Parts smaller than a certain size in pixels are ignored by the graphics card and are therefore not rendered on the screen, for example when zooming out or panning. This is more prominent for graphics cards with lower performance.
Hide edge during rotation when FPS is low
Black edges are not drawn on the screen while the part/assembly is rotated when the "frames per second" (graphics card refresh rate) reaches below a certain value.
Use low quality transparency effects when FPS is low
For graphics cards with lower performance, transparent objects can look very "pixelated". Turn this off if you feel that transparent models are rendered with poorer graphics.
Turn off bold edge display when FPS is low
Black edges are not drawn on the screen when the "frames per second" (the refresh rate of the graphics card) reaches below a certain value.

This controls the basic settings for DWG and DXF import into the ICD drawing and into the 3D scene cross-section (Sketch). There are no specific settings that need to be adjusted.


Hatch accuracy based on part facetting
With this setting active (recommended), you get sharper edges on sectioned objects in the 2D drawing's section views. The views use Precise Mode if the view with the section line also uses that setting.
New BOMs should use 3D scene's Default configuration
With this setting active (recommended), the 2D drawing's bill of materials (BOM) directly reflects the 3D scene's default configuration. When disabled, suppressed items are also displayed in the BOM, and you can place position balloons in views that do not reflect the same configuration as the BOM.
Automatically merge sheet curves with coincident vertices
Sheet curves that align with each other are automatically merged into a group. Recommended disabled.

Show drawing view out of sync dialog
Displays a prompt asking if you want to update the views in the 2D drawing. This prompt appears as a result of modifying the depicted 3D model, or when switching between sheets in the 2D drawing that use different configurations of the depicted 3D scene (which then changes).

Show drawing view of of sync indicators
Displays gray borders around the views that need to be updated. This also appears on section views if the section line is adjusted.


Show warning dialog if target file exists
During DWG and DXF export, you can choose whether to see a warning if you are about to overwrite an existing file.
Display standard view creation dialog when creating new drawing
Automatically launches the view creation dialog when a new 2D drawing is opened.

Use JPEG compression for images
With this setting active, images are heavily compressed during PDF export, resulting in a smaller file size but naturally lower image quality in the PDF file. Disable for better quality in your exported PDF files.
Create PDF content at 100% view scale
Automatically adjusts the scale during PDF export to optimize the quality of colored views and inserted images.
Embed Fonts in IronCAD Drawing integrated PDF for viewing of ICD (larger ICD file size when non-Trye Type fonts included)
The font is saved as part of the ICD file. We recommend keeping this setting disabled, as the file size of the PDF files increases when this function is active.
Embed fonts in exported PDF
The font is embedded only in the PDF file, not in the drawing file (*.icd). This occurs upon export when the 2D drawing is open in IRONCAD.

Reattachment options
Here you manage the default settings for dimensions that have for some reason lost their connection to an edge or point when the drawing is updated.


Here you can add custom properties that can then be applied to parts and assemblies, which in turn can be displayed in e.g. the 2D drawing's BOM or title block.

Here you can check default values for new parts and assemblys that are created.


Read-only Catalog
Controls whether to display a color marker on catalog tabs (ICC files) that are read-only.
Show Tab Colors
Displays the color set via Read-only Catalog Tab Color and Read-only Catalog Tab Text Color in the list above.
Show Lock Icon
Displays a locked or unlocked padlock on the catalog tabs, based on whether the ICC file is read-only or not.

Set Color for
Under Color, the basic colors of many objects in IRONCAD are controlled, e.g. TriBall color active and released, measurement text or new pars default colors. For example:
New ACIS Part
Controls the color of new parts created by import or pulled in from a directory and using the ACIS kernel by default.
New Parasolid Part
Controls the color of new parts created by import or pulled in from a catalog and using the Parasolid kernel by default.
Scene Background
Controls the color of the dimension text background. We recommend white instead of the default grayish-green color for better contrast.
SmartDimensions and Constraints
Controls the color for dimensions in the 3D scene, which is a light green color by default. We recommend black instead for better contrast.
TriBall
The colour of the TriBall when active, taking with it the object(s) that are simultaneously selected. A darker blue colour gives better contrasts and is easier to see, especially when releasing with spaces.