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Emil Rindell
Jonas Bryntesson
Henrik Andersson
2022-03-09
Emil Rindell
Jonas Bryntesson
Henrik Andersson
2022-03-09
There are a number of settings in IRONCAD that are controlled via IRONCAD Options. On this page we go through the most common settings that we recommend looking over. We make most of these settings via the installation of our Swedish Default Customization. But you can of course customize and adjust via this guide to suit you!
IRONCAD Options can be found most quickly via this icon in the Quick Access Toolbar at the top of the program.
Via the Load and Export buttons at the bottom left of the Options window, you can Save and Open the settings you have made. This way you can easily restore or load the settings on another computer.
Via the Search Options button you can search through all the settings under Options.
Show Welcome dialog on startup
Display the welcome dialog (to create new or open existing files) at startup.
Show Welcome dialog when no documents open
Show the welcome dialog when closing all open files.
Number of recent files want to show
Set how many of the last files you worked on will appear in the list in the welcome dialog and in 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.
OBS! Be sure not to save this setting if the warning comes when you open a file, as it will be a permanent setting that must be changed here afterwards.
Precision displayed in dialogs
The number of decimals in dialog boxes; reduce if necessary to 2 or 1. In dialog boxes, however, you can advantageously see more decimals than directly in the graphic (below).
Dimension precision
The number of decimals directly in the 3D graphic; please 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
Checks the size of dimensions and other text in the 3D scene; feel free to increase from 15 to 20 or 22 (looks different 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 activated, you get a reminder to save the file every X number of minutes, which you set numerically in the box next to it.
Track open file modified by others
If several people are working on shared files (external links) and make changes, they may receive a message that a particular file has been changed by someone else. The file must then be manually closed and opened to read in these changes. Set the desired check interval in seconds.
Enable camera Look At during editing
With this setting active, an automatic rotation of the camera position towards the grid is obtained when editing the cross-section (Sketch). Turn off if you do not want an automatic camera rotation when you select Edit Cross-section. The setting below resets the camera settings when 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 when 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
Corresponding setting for so-called "helix" shapes - i.e. screws or springs. Can be advantageously set to 10 as standard
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
Please enable the ability to snap and drop models from directories against "Ghost" objects, is off by default but smoother if enabled.
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 program should automatically suggest 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). Even here, many start to change so that you automatically get the file name adjusted to the current number (Part Number) and description (Description) that is used on what is first in the history tree (when saving the file) or on what is selected when saving an external link or copy.
Keep Part/Assembly order when creating assembly or copying them
Turn off the option because it works better that the order is determined by how you selected the objects, not what order they were in the tree before you selected them. If you have been working with IRONCAD for many years, this setting may seem unusual at first.
When dropped on pattern or linked feature
Checks if you should automatically get linked copies of what you drop from a directory on all the same forms as the one you drop on. For example, if you drop a screw on a linked hole, then 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)
Is about using the [Shift] key or not, when snapping to other geometry. With this option enabled, it means using the [Shift] key to avoid snapping to other geometry, which many people find backwards.
Maintain geometry of adjacent curves when dragging profile curve
When dragging with the Shape handles, you can control how connecting lines other than 90-degree angles are handled. The default setting (active) reduces the length of the line you draw, extends and maintains the angle (see right line) of the two connecting lines:
Off, maintains the length of the line being drawn, it forces connecting lines to be extended but also possibly to change the angle (see line to the right):
Show edit toggle icon upon selection
Control the display of the white button that switches the handle type between either red round Sizebox handles or red angular Shape handles. Remember that the [TAB] key on the keyboard has the same function!
Automatically switch to next sizebox handle value after enter
Means to automatically jump to the next handle when pressing [Enter]. Most people keep this feature turned off.
Disable Symmetrical Handle Toggle
Means to turn off the Symmetrical Handle Toggle button that appears inside the handles and locks them symmetrically over time. Tip! Right drag the Sizebox handle for symmetry.
Disable Symmetrical... enabled:
Disable Symmetrical... off:
Enable Dynamic Sizebox Dimension Display
The measurement box (Sizebox Dimension) is attached to the mouse pointer, instead of in the middle between the handles. We have left this active, as many people have asked for just such a feature.
Enable Dymanic Sizebox... enabled:
Enable Dynamic Sizebox... off:
Automatically add position dimension on dropping feature
Automatically adds one or two SmartDimension dimensions from the nearest edge(s), when dropping features from a catalog. Same principle as for 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
Control whether you want Number or Distance/Angle to be selected first. Many people want Distance/Angle, because you can easily type a large number, say 1000, 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
Maintains the selection on the item that is released from a catalog.
Drop assembly/part into selected assembly
The object dropped in the 3D scene will automatically become part of the smst that is selected.
Show design variation dialog when dropped object
Displays the dialog for Design Variations (parameterized 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 from a directory.
Show resize shape dialog
Displays the Resize Shape dialog box. This means that the new part is resized to fit the camera view.
Show part name tooltip
Show or not show the white label that appears at the mouse pointer when clicking on objects in the 3D scene.
Orbit about cursor location
Means that you rotate around an object if the mouse arrow is on top of that object. Otherwise it is 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
This means that you zoom in towards the position of the mouse cursor on the screen. Turn it off and you zoom straight in/out instead.
Reverse zoom direction
This means that you reverse the zoom based on the scroll wheel, instead of zooming in, you zoom out when you roll the wheel in one direction.
Mouse Gesture
Provides the ability to start and execute commands via mouse gestures (painted as orange lines in the graphic) when holding down BOTH the left and right mouse buttons simultaneously. Here you can disable this feature if you accidentally access it or don't want to use it at all. Also the time for simultaneous left-and-right press before the mouse gesture is activated and information (popup mouse gesture list) about the available mouse gestures.
Working directory
Is the folder suggested when saving and opening files directly after starting the application. If you have started working with files in a specific project, this is the folder that opens when you choose to open files. If you have saved files in another folder, the folder in which you last saved is always shown.
Template directory
The path to 3D, 2D, BOM templates in IRONCAD. This path can be placed on a common file server if there are several people working in IRONCAD and using common 2D drawing templates.
Tips! Or put templates in Shared Documents to not be hampered by IT/rights restrictions settings.
Default path for templates (from 2020 PU1 SP1):
C:\Users\*YOUR USER*\AppData\Roaming\IronCAD\IRONCAD\*22.0 AND FUTURE*\en-us\Template
Previous versions were located here:
C:\Program Files\IronCAD\*2020 AND BACK*\AppData\en-us\Template
Display Sheet Metal feature shape handle as default
Checks whether to use the red round Sizebox handles (at Off) or the red square Shape handles (at On) by default. The difference is that you either stretch (rescale) all lines at once (Sizebox) or work on them individually (Shape).
Display Sheet Metal unfolded direction arrow
Choose whether to have an arrow showing in which direction the sheet is spread.
Set new unfolded Sheet Metal part as "Included in BOM"
Checks whether the extended plate should also automatically use the Include in BOM setting and thus appear in the parts list in the 2D drawing. This in combination with the bottom setting to copy over Part Properties to the extended sheet is probably related in most cases, either both are active or both are turned off.
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 spreading a sheet, you can manually select certain other objects to be visible (not suppressed) for each object afterwards. When you then spread again, IRONCAD has "forgotten" which batches were not suppressed. But with this setting you can have a propagation remember what is not suppressed. The setting avoids having to select it every time you propagate.
Display stock selection dialog on dropping stock
Displays the plate table when a new plate (Stock) is released into the scene.
Use Stock name as Material
The name of the plate is entered as a material under Material properties.
Use Stock Name as Description and Code as Material
The name of the plate is entered in Description (under Part Properties) and the material code under Material properties.
Auto-Maintain bend alignment for newly created bend
This setting controls how First Bend Stock is handled when the bend angle is changed. It is similar to the settings for Second Bend Stock.
With the setting off (not recommended), the length value of the First Bend Stock will change as the angle changes, in order to maintain the total amount of material (even if the angle changes). This means that material is added between the buck and the connecting log when the angle of the buck is changed. Enabling this setting instead makes it more predictable in that no extra material is added between the buck and the next log when the angle of the buck is changed. Most often you want First Bend Stock Length set to 0 mm, just like with Second Bend Stock Length. This means that the buck sits close to the edge you dropped it against and no extra material squeezes in between.
Bend line angle in drawing measured down from 180 degrees
Some bending machines count down from 180° instead of up from 0°. With this setting, the bending 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 the In Bend and Out Bend automatically "skew in", so you don't have to pull the Shape handles (or via numbers under Bend Properties, Corner Reliefs) to change from flat end to a "smooth transition" at the ends:
Function set as Active, see how the ends are not "flat" (default setting from 2020):
Off (as it was before v2020), most prominent on the right end (Left according to reliefs):
Bend Reliefs
Controls the standard shape and dimensions of the release tabs at the end of the bucks, which are also accessed individually via the red square Relief handles on a buck.
Second Bend Stock Length
At each end of a buck there is an option to extend it straight out from the buck end, we call this the "buck length extension". The length extension that is on the opposite side of the edge the buck is attached to is called the Second Bend Stock. There are four different options for how this length extension is calculated when the bend angle is changed; Flange, Tangent, Inner Sharp and Outer Sharp. There are also three options under Update Behavior that control how, or if at all, this length allowance is changed when the bend angle changes; Default, Maintain unfolded length when changing angle and Maintain specified length.
Create punch and forming constraints
Automatically inserts 2 dimensions against the nearest edges you dropped the hole/punchphom, 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 lock the shape to the edges of the sheet. These settings can be accessed at any time via the right-click menus of the target.
Auto-Constraint bends
Automatically creates a constraint for each check against the edge the check is released. When edges are moved, the check follows, but it is never extended (reshaped).
Auto-Associate to attached entity
Instead of creating a contraint property, each new feature, created when dropped from the SheetMtl directory on a sheet edge, is associated against the edge. The advantage of this setting is that bucks and sheet parts are automatically extended when the edge they sit on is extended. This saves a lot of time!
See more here: https://www.youtube.com/watch?v=GlyWx6Kl_SE&feature=youtu.be
Advanced Options
Via the Advanced Options button... 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 controls how large the gap between the parts of the plate should be by default, e.g. when using the Snap to point for corner option on a Relief handle.
New part size - controls the default size of new plates created by dropping 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 directory) should be positioned when released so that they are affected by a check mark. Active = In relation to the extended plate (recommended). Off = Directly positioned on the buck (not in the plane), most likely without showing any dimension from an edge, making it more difficult to reposition (not recommended).
Bend corner treatment - controls the basic setting for the gap that occurs when using the Snap to Point for Corner function on a Shape handle.
Here you can select the standard thickness of your sheet from a list. The sheet type selected in the list is used when you drag a new sheet (Stock) into the 3D scene. The active sheet type is displayed at the top. Below the list are two settings for file paths that list all plate thicknesses and plate 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)
When working with point clouds, this setting is important to activate. For some add-in functions such as DDM it is important NOT to have this function active.
Driver type (graphics engine)
IRONCAD offers different options that may be suitable for different graphics cards. In case of graphics problems, try changing the graphics engine from OpenGL to DirectX. This can make a big difference for graphics cards with poorer performance.
(NOTE: Close all open documents first).
Display List
Segment is said to work best in general, but it is computer dependent and you should therefore test the three options, Auto, Segment or Geometry.
Compute mass for part and assembly automatically
This setting affects regeneration to calculate the mass (weight) of batches and assemblies. Recommended off to save performance.
Auto preview when edit feature
With this active, a preview is shown directly when editing a feature. E.g. a Blend. To save performance it is recommended to turn this off.
Do model check after feature command
Run a check on the feature created. Recommended 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 should speed up the time it takes to open files. However, you can turn it off if you have graphics problems, as the file's saved graphics data (cache) is automatically reset immediately when the file is opened.
Use Visual Load when Opening Files
Use a function that opens the graphical part of an ICS file in a fraction of the time it takes the whole file to open. During this time, tools other than the camera (zoom and rotate) cannot be used.
Hide small parts automatically
Parts smaller than a certain size in pixels are ignored by the graphics card and are therefore not drawn on the screen, e.g. 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 transparenct effects when FPS is low
For graphics cards with lower performance, transparent objects can look very "pixelated". Turn this off if you find that transparent models are drawn 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.
Basic settings for DWG and DXF import to the ICD drawing and to the 3D scene cross-section (Sketch) are checked here. There are no special settings that need to be adjusted.
Hatch accuracy based on part facetting
With this setting active (recommended), sharper edges are obtained on cut objects in the 2D drawing's cut views. The views use Precise Mode if the view with the intersection line also uses this setting.
New BOMs should use 3D scene's Default configuration
With this setting active (recommended), the 2D BOM directly maps the default configuration of the 3D scene. With the setting off, suppressed objects are also displayed in the BOM, but you can also put pos balloons in views that do not depict 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 off.
Show drawing view out of sync dialog
Displays a window asking if you want to update the views in the 2D drawing. This question comes as a result of changing the 3D model being imaged, or switching between sheets in the 2D drawing that use different configurations of the 3D scene being imaged (which then changes).
Show drawing view of of sync indicators
Shows grey frames around the views that need to be updated. Also appears on section views if the section line is adjusted.
Show warning dialog if target file exists
For DWG and DXF export, you can choose 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, the images are heavily compressed when exporting to PDF, which results in a smaller file size but also, of course, a lower quality of the images in the PDF file. Turn it off for better quality of your PDF files in exported PDF files.
Create PDF content at 100% view scale
Automatically adjusts scale on PDF export to optimise the quality of coloured views and loaded 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 that you have this setting disabled as the file size of PDF files increases when this feature is active.
Embed fonts in exported PDF
The font is only inserted in the PDF file, not in the drawing file (*.icd). This happens on export when the 2D drawing is open in IRONCAD.
Reattachment options
This handles the basic settings for dimensions that for some reason have lost their connection to an edge or point, when the drawing is updated.
Here you can enter your own properties which can then be added to parts and assemblies, which in turn can be displayed in e.g. the 2D drawing's parts list or drawing header.
Here you can check default values for new parts and assemblys that are created.
Read-only Catalog
Controls whether to see a color mark on directory tabs (ICC files) that are read-only.
Show Tab Colors
Displays the color set via Read-only Catalog Tab Color as well as Read-only Catalog Tab text Color in the list above.
Show Lock Icon
Displays a locked or open padlock on the directory 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
Control the colour of the matte text background, which we recommend is white instead of the default greyish-green colour, which provides better contrast.
SmartDimensions and Constraints
Controls the color of the 3D scene's target set, 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.
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