How Do You Change PCB Board Size in Ultiboard?
To change PCB board size in Ultiboard, edit or replace the geometry on the Board Outline layer. For a simple rectangle or circle, use Tools > Board Wizard. For an enclosure-controlled shape, import a DXF into the Board Outline layer. For a custom shape, draw a polygon on that layer. Afterward, check the origin, every corner, component and copper clearances, mounting holes, DRC results, and the exported Gerber outline.
This guide follows the three outline methods documented by NI and then continues through the checks needed before fabrication. That second part matters: changing a line on screen is easy; proving that the resized PCB still fits, routes correctly, and can be manufactured is the real job.
What Defines PCB Board Size in Ultiboard?
In plain language, the Board Outline is the cutting path that tells the PCB manufacturer where the finished board begins and ends. Its outermost X and Y coordinates determine the overall length and width, while arcs, notches, and internal cutouts define any non-rectangular geometry.
The outline is not the same as the drawing sheet, grid, copper pour, keep-out, or silkscreen border. Enlarging the workspace does not enlarge the PCB. Moving a copper shape does not change the routed board edge. You must work on the Board Outline layer and make sure the final contour represents one unambiguous physical profile.
This distinction matters because a fabricator reads manufacturing output, not the visual impression of your Ultiboard workspace. If the actual outline is missing, open, duplicated, or on the wrong output layer, the board may be placed on hold even though the design looked normal in the editor.
Which Board-Outline Method Should You Use?
Choose the method from the source of truth for the board’s mechanical shape. Do not redraw a complex enclosure shape by eye when a mechanical DXF exists, and do not import a complicated file when the board is only a plain rectangle.
| Situation | Best Method | Why | Main Check |
|---|---|---|---|
| Simple rectangle or circle | Board Wizard | Fast, repeatable dimensions | Correct units and layer count |
| Shape controlled by enclosure CAD | DXF import | Preserves mechanical geometry | Scale, layer mapping, and origin |
| Simple custom outline with a few vertices | Polygon | Direct control inside Ultiboard | Exact coordinates and closed corners |
| Small adjustment to an existing verified shape | Edit outline properties where supported | Avoids rebuilding the whole profile | Recheck every affected clearance |
Menu names and editing behavior can differ between Ultiboard releases. The verified NI workflow is Board Wizard, DXF import, or a polygon on the Board Outline layer. If your version exposes additional geometry properties, use them only after confirming that the selected object is the real board outline.
What Mechanical Information Should Be Ready First?
Before changing the board, write down the mechanical constraints that the PCB must obey. At minimum, confirm the finished length and width, measurement units, corner radii, mounting-hole centers, connector locations, keep-out areas, maximum component height, and the datum used by the enclosure drawing.
A useful datum is a stable point from which every other location can be measured, such as the lower-left board corner or the center of a mounting hole. Without a shared datum, a PCB designer and mechanical engineer can both use correct dimensions but still place the connector in different locations.
For example, suppose the enclosure allows a 90 mm by 60 mm board and locates four holes 3 mm from each edge. If you shrink only the outline from 100 mm by 70 mm to 90 mm by 60 mm, the old holes may remain 8 mm from the new edges or even fall outside the board. The board dimensions are correct, but the mechanical interface is wrong.
Prepare the enclosure DXF or STEP file, a dimensioned drawing, the intended units, tolerance notes, and any connector or switch alignment requirements. If another team owns the enclosure, obtain written approval of the datum and revision before releasing fabrication data.
How Do You Select and Delete the Existing Outline?
NI’s documented starting point for a replacement outline is to delete the default or old outline. Enable the Other Objects selection filter, double-click Board Outline in the Design Toolbox to activate that layer, select the existing outline, and press Delete.
If clicking the edge selects a trace, component, or other object, stop and verify the active layer and selection filter. Deleting random geometry until the border disappears can damage the layout while leaving the real outline intact.
Before deletion, save a new design revision. Record the original dimensions and take note of the reference point. This gives you a clean rollback and makes it possible to compare old and new coordinates after the change.
How Do You Set a Simple Size With Board Wizard?
For a straightforward rectangular or circular board, delete the old outline and open Tools > Board Wizard. Follow the wizard, choose the required board shape and dimensions, and confirm the board technology or layer settings shown by your Ultiboard version.
- Save a new revision and record the required finished dimensions.
- Activate the Board Outline layer and remove the old outline.
- Open Tools > Board Wizard.
- Select the shape, units, dimensions, and applicable layer configuration.
- Finish the wizard and measure the generated outline.
- Reposition or verify the reference point before moving components.
Do not treat the wizard’s completion screen as final approval. It creates geometry; it does not prove that connectors, holes, copper, and routed traces still satisfy the new edge locations.
How Do You Import a Mechanical Outline From DXF?
Use DXF when the enclosure or industrial designer owns the board profile. NI documents DXF outline import for the Power Pro edition, so first confirm that your Ultiboard edition supports the function.
- Clean the mechanical drawing so it contains one intended outer contour and clearly identified cutouts.
- Delete the existing Ultiboard outline.
- Select File > Import > DXF and choose the approved file.
- Choose Merge import data into existing layers.
- Map the correct DXF geometry to Board Outline.
- Select the same units used when the DXF was exported.
- Use Design > Set Reference Point to place the intended design origin.
- Measure a known dimension and compare it with the mechanical drawing.
The known-dimension check catches the most expensive DXF mistake: a unit mismatch. A 3.5-inch dimension interpreted as 3.5 mm is obviously wrong when measured, but it may not be obvious from a zoom-to-fit view.
Remove title blocks, dimension arrows, construction lines, and duplicate contours before they become board geometry. Ask the mechanical owner which contours are the outer profile, routed slots, internal cutouts, and reference-only shapes.
How Do You Draw a Custom Polygon Outline?
For a custom shape with a manageable number of corners, activate the Board Outline layer and use Place > Shape > Polygon. Start from a known reference point, enter or place each vertex in order, and return exactly to the first point to close the contour.
NI recommends preparing a list of X and Y coordinates for more complex polygons. This turns an improvised mouse drawing into a checkable engineering definition. Work clockwise or counterclockwise consistently so that missing or repeated vertices are easier to spot.
For example, a 60 mm by 40 mm rectangle with a 5 mm corner notch might be defined by the sequence (0,0), (60,0), (60,35), (55,40), (0,40), then back to (0,0). The final coordinate must meet the starting coordinate; looking close at normal zoom is not enough.
How Do Units and the Reference Point Affect the Result?
Units control scale, while the reference point controls position. A board can have the right shape but the wrong size if inches and millimeters are mixed. It can also have the right size but the wrong relationship to components and holes if the origin changes unexpectedly.
After any import or redraw, measure at least one long dimension and one local feature. Then check a known hole or connector coordinate from the agreed datum. This two-level check catches both global scale errors and local alignment errors.
Do not move the origin merely to make screen coordinates look tidy. First ask what downstream files use that origin. Pick-and-place data, assembly drawings, test fixtures, mechanical drawings, and programming fixtures may rely on it. If the origin must change, notify every downstream owner and regenerate affected outputs.
What Can Go Wrong When You Reduce Board Size?
Shrinking a board changes available area and every distance to the nearest edge. Components may cross the profile, copper may violate edge clearance, traces may have no legal rerouting path, mounting holes may lose support, and connectors may no longer align with an enclosure opening.
| Failure | What You May See | Why It Matters | Required Action |
|---|---|---|---|
| Component outside outline | Body or courtyard crosses edge | Part cannot be assembled or board cannot fit | Move part and recheck mechanical access |
| Copper too close to edge | Trace, plane, or pad near route line | Routing tolerance can expose copper | Apply fabricator edge-clearance rule |
| Mounting-hole breakout | Hole or annular ring near edge | Weak material and plating risk | Move hole or enlarge board with approval |
| Broken return path | Plane neck-down after rerouting | Signal integrity or EMI can worsen | Review return currents, not only DRC |
| Duplicate/open outline | Gerber viewer shows odd segments | Fabricator cannot infer one route path | Remove duplicates and close every corner |
The important lesson is that DRC is necessary but not sufficient. A rule checker can find configured violations; it cannot know that a USB connector was supposed to remain centered in an enclosure opening unless that mechanical requirement is represented and reviewed.
How Do You Check Components, Copper and Mounting Holes?
Check from the board edge inward. First inspect the physical body and courtyard of every edge connector, switch, LED, antenna, heatsink, and tall component. Next inspect copper features: traces, planes, pads, vias, test points, and exposed-metal features. Finally inspect holes, slots, and board-edge support.
Use the clearance values agreed with the fabricator rather than a generic number copied from another design. Required copper-to-edge spacing depends on the routing process, scoring, plated edges, controlled-depth features, tolerance, and product reliability needs.
For assembly, verify that pick-and-place nozzles, selective-solder fixtures, depaneling tools, and test probes still have access. A smaller bare board may be manufacturable but difficult to assemble or test. For support with these checks, QFPCB’s PCB design service can review the layout-to-mechanical relationship before files are released.
How Do You Verify a Closed Board Outline?
A valid outer outline should form one continuous closed perimeter with no microscopic gaps, overlapping segments, accidental branches, or duplicate shapes. NI identifies unconnected corners as a common board-outline error and recommends zooming in closely at every corner.
Run the available design checks, but also perform a visual corner-by-corner inspection at high zoom. Check where lines meet arcs, where imported DXF segments join, and where the last polygon vertex returns to the first. If the viewer fills or recognizes the shape inconsistently, assume the geometry needs repair.
Internal slots and cutouts should be separate, intentional closed contours and clearly identified in the fabrication notes. Do not rely on a keep-out shape or a filled graphic to communicate a routed opening.
How Should You Review Gerber and Drill Output?
The manufacturing files are the final truth. Regenerate the Gerber and drill files after resizing, open them in an independent viewer, and confirm that the outline has the intended dimensions, orientation, origin relationship, slots, cutouts, and hole locations.
Overlay the copper, solder mask, silkscreen, drill, and outline layers. Look for copper outside the profile, clipped reference designators, holes outside the board, duplicate outlines, and a mismatch between plated and non-plated mechanical holes. Compare the viewer’s measured length and width with the approved drawing.
If assembly is included, also regenerate centroid data and assembly drawings because a changed origin or moved component can make older files inconsistent. A prototype PCB assembly run is useful when the mechanical change is substantial and enclosure fit must be proven before volume production.
Ultiboard Board-Resize Release Checklist
Use this checklist before sending the revised design to a manufacturer or another team:
- The approved finished length, width, shape, units, and tolerance are recorded.
- The enclosure drawing and PCB use the same datum and revision.
- Only one intended outer Board Outline exists.
- Every line-to-line and line-to-arc corner is connected at high zoom.
- All routed slots and internal cutouts are closed and identified.
- Mounting-hole coordinates and edge distances match the mechanical drawing.
- Connectors, switches, LEDs, antennas, and tall parts still align with the enclosure.
- Copper, pads, vias, planes, mask, and silkscreen satisfy edge rules.
- Routing and return paths were reviewed after component movement.
- DRC was rerun with the intended fabrication constraints.
- Gerber and drill files were regenerated and measured in an independent viewer.
- Assembly, centroid, drawing, and 3D files were regenerated where affected.
- The release package contains no old files with the same name.
- A second person compared the final output with the approved mechanical drawing.
FAQ About Changing PCB Board Size in Ultiboard
Can I change PCB size by changing the workspace or grid?
No. The workspace and grid help you navigate and place objects; the Board Outline defines the physical PCB profile.
Why can I not select the existing board edge?
Confirm that Other Objects is enabled in the selection filter and that Board Outline is the active layer. You may otherwise be clicking a different object near the edge.
Which method is best for an enclosure-controlled board?
Use an approved mechanical DXF when your Ultiboard edition supports it. Map only the intended contour to Board Outline, match the units, set the agreed reference point, and verify a known dimension.
Can I drag the outline until it looks correct?
A visual adjustment may be acceptable for an early concept, but a released design needs controlled dimensions and coordinates. Measure the final shape and compare it with the mechanical drawing.
Does changing the outline automatically move components and holes?
No. Treat the outline change and the layout update as separate tasks. Recheck every edge-sensitive component, mounting feature, copper area, and route.
How do I know whether the DXF scale is correct?
Select the matching import units, then measure a dimension whose value is known from the source drawing. Do not trust zoom-to-fit as a scale check.
Why does the fabricator report an open outline?
Two segments may look connected while their endpoints differ slightly. Zoom into every corner, remove overlaps or duplicates, close the contour, regenerate the Gerber, and inspect it again.
Should the board outline be added to every Gerber layer?
Fabricator preferences differ. Provide one clear profile layer and follow the manufacturer’s file instructions. Avoid multiple conflicting outlines across the package.
What files should be regenerated after resizing?
At minimum, regenerate Gerber and drill data. If the origin or component positions changed, also regenerate centroid data, assembly drawings, 3D/mechanical exports, and any fixture coordinates.
Should I prototype after a major size change?
Yes when enclosure fit, connector alignment, assembly access, thermal behavior, antennas, or test fixtures may be affected. A prototype verifies the interfaces that software rules cannot fully understand.
Need PCB Design and Prototype Review?
Before requesting a quote, send the Gerber and drill files, stackup, finished board dimensions and tolerance, DXF or STEP enclosure data, fabrication notes, and the approved mechanical drawing. For assembly, also include the BOM, CPL, assembly drawings, test requirements, and any programmed-device notes.
QFPCB can support PCB assembly and review whether the resized layout is ready for a prototype build. Use the contact page to share the package and identify the mechanical features that changed. A clear revision note helps engineering compare the new release with the previous board instead of guessing what moved.
