Between the two packages there are five tools that actually look at draft or undercuts. DFMXpress, the one most people name first, is not among them, which is where this has to start.
One of the five gets close enough that it belongs up front: Fusion's Design Advice, which is part of a paid extension. The other four will show you draft and undercuts without telling you whether the part is moldable. They ask you for the pull direction, they ask you for the threshold, and then they color the model according to what you gave them.
Here is what each one covers, and what a written check returned on the same part.
What does DFMXpress check for injection molding?
Two rules. Minimum wall thickness and maximum wall thickness.
That's the complete Injection Molding rule set in the SOLIDWORKS documentation. The minimum-wall rule carries a recommendation of 2.0mm, on the grounds that walls which are too thin cause filling problems and develop high molding stresses. The maximum-wall rule is there to avoid cooling problems, sink marks, internal voids and long cycle times.
Draft isn't in the set. Undercuts aren't in the set.
DFMXpress is the button most people have in mind when they say their CAD package checks manufacturability. You go to Tools > DFMXpress, pick a rule set under Manufacturing Process (Mill/Drill only, Turn with Mill Drill, Sheet metal, or Injection Molding), and run it. Under Settings, the rule parameters are values you type in.
So a part can pass DFMXpress under the Injection Molding rules with every vertical face at zero draft and a side-action undercut sitting in it. Those two checks were never in the rule set to begin with.
What the draft and undercut tools give you
Colors, a count per category, and a number under the pointer.
SOLIDWORKS Draft Analysis is on the Mold Tools toolbar. You select a planar face, a linear edge, or an axis to define the direction of pull, enter a reference draft angle, and click Calculate. With Face classification on, every face is sorted into a category, colored, and counted. The results stay visible in the graphics area after you close the dialog and update in real time as you change the geometry, and you move the pointer over the model to display the draft angle in that area.
SOLIDWORKS Undercut Analysis sits on the same toolbar and finds trapped areas that can't be ejected and therefore need a side core. It takes a plane, face or edge as the direction of pull, or coordinates, or a parting line instead of a direction. Faces come back sorted into undercut categories, each in its own color. The documentation notes that it works on solid bodies and doesn't work on surface bodies.
Fusion 360 puts Draft Analysis in the Inspect panel. Select the bodies and an axis, and you get a color gradient; the Autodesk documentation says you can use it to evaluate positions for a parting line or to find areas of zero draft or undercuts. Accessibility Analysis, in the same panel, colors a body green where regions are accessible from a particular plane and red where they are not, which is the trapped-geometry question asked from the other side.
All four of those are real analysis and they come with the license. The shape of what they produce is a colored model, a count per category, and a value if you hover. What none of them hands you is a written list of findings with the number each one failed against, which is the thing you'd paste into the message where you ask your molder about face 12.
The fifth tool, and it costs extra
Fusion's Design Advice sits in a different category, and any comparison that leaves it out isn't worth reading. It comes with the paid Fusion Design Extension, which is most of why it comes up less often than it should.
Per Autodesk's documentation, you select a solid body and the pull direction, click Analyze, and it returns summary cards for thickness regions that fall outside the range or exceed the variation limit, undercut regions that will interfere with ejection, faces that don't meet the minimum draft angle, and knife edges below the threshold. Each alert type opens a detail tab carrying a list of alerts and recommendations, and you can select one to highlight it in the canvas or ignore it to filter it out.
The thresholds don't come from you. Design Advice uses the Plastic Rule assigned to the component that contains the body, and the plastic material along with the thickness and draft rules are inherited from that rule.
So of the three things the free tools leave undone, Design Advice does two. The threshold comes from material data, and the output is a list. It still asks you for the pull direction, and it still needs the model open in Fusion with an extension license behind it.
The same question, run as a written check
I ran a test part measuring 50 x 50 x 100mm with 15 faces as polycarbonate for injection molding. Three times, to see whether the number held: 3.1 seconds, then 2.4, then 2.3.
Twenty-one findings. Fourteen of them are geometry:
- Two faces at exactly 0.0 degrees of draft, faces 3 and 12, against the 2.0 degree smooth-surface minimum the check applies to polycarbonate. Those two are the largest faces on the part, 7,539.8 mm² each.
- Ten wall sections over the maximum, ranging from 3.85mm to 5.03mm, compared against 3.81mm for PC.
- Two undercut faces, 0 and 2, each undercut by 1.2 degrees.
The other seven are defect risks derived from the geometry. Sink marks came back at 0.7 probability and high severity, citing the ten thick sections as the cause and naming the affected faces individually: 0, 2, 3, 4, 5, 7, 8, 9, 10, 12. Warpage came back low, with a wall thickness ratio of 1.04. The tooling model put the mold at 14,000 USD at moderate complexity for a US shop with no slide cores added, alongside a 20.3 second cycle, 177 parts per hour and a predicted yield of 93 percent against an industry range of 95 to 98 percent. The badge at the top of the report reads Optimization Recommended.
Insight
The two undercut faces are the ones worth dwelling on. Set the reference angle to 2.0 degrees, which is what polycarbonate asks for, and SOLIDWORKS sorts faces into Positive draft, Requires draft or Negative draft, with extra categories for straddle and steep faces. A face undercut by 1.2 degrees is not below the negative reference, so it lands in Requires draft, wearing the same color as the two faces sitting at 0.0 degrees. One of those pairs needs draft added and the other pair is undercut. The check filed the undercut pair as low severity with a note that they may not require action, because 1.2 degrees falls inside the band where a side action probably isn't warranted.
Tip
The cost figures here come from a region and complexity model built into the app. They are estimates, not a shop quote. The part is a synthetic test model.
Where the approaches actually differ
Start with what's the same. None of these tools finds the pull direction for you. SolidWorks makes you pick a face, edge or axis every time you run the analysis, Design Advice asks for it too, and the check takes the model's +Z axis, which means an import that arrived in some arbitrary orientation gets measured against a pull you never intended. If you haven't settled which way the mold opens on this part, that decision comes before any of them is any use, and it's worth reading how part orientation sets the mold opening direction before you trust a number from any of them.
The threshold is where the free tools come apart from the other two. SOLIDWORKS Draft Analysis asks you to type a reference draft angle, and the colors mean whatever you typed. The check above compared against 2.0 degrees because that's polycarbonate's smooth-surface minimum in its material data, and it compared the walls against 3.81mm for the same reason. Switch the same file to ABS and the wall ceiling drops to 3.56mm on its own, while the draft minimum stays at 2.0 degrees for both resins. I ran it both ways instead of assuming, and on this part the flagged set doesn't move at all: the thinnest flagged wall is 3.846mm and was already over both ceilings. What the material data buys you is the right ceiling on the part where a wall does sit between the two.
| What you want | SolidWorks tools | Fusion, base license | Fusion Design Advice | A written check |
|---|---|---|---|---|
| Faces with insufficient draft | Colored and counted | Color gradient | Alert list | Face number and measured angle |
| Where the threshold comes from | What you typed | What you set | The component's Plastic Rule | The selected material's data |
| Undercut locations | Color classification | Green and red regions | Alert list | Face number and angle |
| How serious a given undercut is | Category set by your reference angle | Position on the gradient | Alert list, no documented severity ranking | Severity band, noted when action is unlikely |
| What the findings lead to | Not covered | Not covered | Recommendations to resolve | Sink mark risk on the named faces, part-wide warpage, plus a tooling and cycle model |
| Where the file has to be | Open in SolidWorks | Open in Fusion | Open in Fusion, extension license | Read from STEP on your computer |
Reading that table honestly
Design Advice closes most of the gap the free tools leave. What remains after it is narrower than a sales pitch would suggest, and it comes down to two things.
One is what a finding connects to. Design Advice returns recommendations for resolving an alert, which is advice about the geometry itself. The written check returns the defect risk the geometry implies, the faces sink marks are attributed to, and a tooling and cycle model for the same part.
The other is where the file has to be. Every one of these tools needs the model open in the package it belongs to and a license to open it, DFMXpress included, and Design Advice needs an extension on top of that. A colleague's STEP file, no seat of the package it came from, and a deadline is a combination none of them cover, which is the same structural gap that shows up when people try to get DFM answers out of ChatGPT instead.
How to run this on your own file
Drop the STEP or STP straight in. There's no import step and no CAD package in the way, so the file you were sent is the file you check, and it stays on your computer while it runs.
Pick the material first. The material supplies the wall ceiling and the draft minimum that the run gets judged against. If the file holds more than one solid, settle which body gets analyzed first, since the default is the largest one by volume.
Tip
Your CAD files are never uploaded. STEP and STP files stay on your computer through the analysis, and only the defect findings are processed by AI and synced to your account.
Frequently asked questions
Does SolidWorks check draft angles and undercuts?
Yes, through two separate tools on the Mold Tools toolbar. Draft Analysis asks you to select a planar face, linear edge, or axis to define the direction of pull and to type a reference draft angle, then classifies each face into a color category and counts them; you move the pointer over the model to read the angle in a given area, and the result stays live in the graphics area after you close the dialog. Undercut Analysis finds trapped areas that need a side core, takes a plane, face or edge as the direction of pull or a parting line instead, and works on solid bodies only. Neither one is part of DFMXpress, which is the tool most people mean when they say their CAD package checks manufacturability.
What does DFMXpress check for injection molding?
Two rules: minimum wall thickness and maximum wall thickness. That is the entire Injection Molding rule set in the SOLIDWORKS documentation. The minimum-wall rule carries a recommendation of 2.0mm, and the maximum-wall rule exists to avoid cooling problems, sink marks, internal voids and long cycle times. Draft angle is not in the set and neither are undercuts, and the rule parameters under Settings are values you type in yourself. A part can pass DFMXpress under the Injection Molding rules with every vertical face at zero draft.
Can Fusion 360 find undercuts?
In three different ways, and one of them costs extra. Draft Analysis in the Inspect panel displays a color gradient once you pick an axis, and the Autodesk documentation says you can use it to find areas of zero draft or undercuts. Accessibility Analysis in the same panel colors a body green where regions are accessible from a chosen plane and red where they are not. Design Advice, which is part of the paid Fusion Design Extension, goes further: you select a solid body and the pull direction, and it returns alert cards for thickness, undercuts, draft and knife edges, with the thresholds taken from the Plastic Rule assigned to the component rather than typed in by you.
What draft angle does a check use for polycarbonate?
The check on this part compared against 2.0 degrees for a smooth surface, with 3.0 degrees for a textured one, which are the figures in its material data for PC. Published guidance for molded plastics puts the absolute floor lower than that and the comfortable range around 1 to 2 degrees per side, so 2.0 sits at the conservative end. The number matters because it is the input the free CAD draft tools do not supply: SOLIDWORKS Draft Analysis asks you to type a reference draft angle, and whatever you type is what the colors mean. The distinction also stops mattering at zero, which is what two faces on this part measured.
Do you still need a CAD license to check a STEP file for moldability?
For the SolidWorks and Fusion tools, yes, and the part also has to be open in that package on a computer that runs it. Fabdose reads the STEP or STP file directly on macOS or Windows without a CAD license, keeps the file on your computer, and returns a written list of findings with the face number, the measured value, the threshold it was compared against, and the position. On the test part in this post, three runs took 3.1, 2.4 and 2.3 seconds.
Analyze your STEP file on your computer. Your CAD file is never uploaded.
Download Fabdose Free