Skip to content
Knowledge base

How do I read the CAM iX log file and fix 'no machining principle found'?

How to read the CAM iX report per part, find the part causing the error and fix 'No machining principle available' step by step.

Short answer: Generate the CNC programs with the Create log file option ticked and expand the report down to part level: every operation should show a machining principle. The message 'No machining principle available' means no principle fully matches. Then check, in order, the machine, the workflow, the principle's conditions and the material's formatting class.

Information

Applies to

  • imos iX 2017 and later with CAM iX
  • Module: imos CAM iX, imos Manager
  • Integrations: the postprocessor of your CNC machine
  • Last reviewed: October 2026

Creating the log file

  1. In the imos Manager, right-click the article that contains the part.
  2. Choose Generate CNC programs.
  3. Tick Create log file.
  4. Click Start. Previously generated CNC files are overwritten.

Reading the report

  1. The report is a tree structure per order. Expand it down to part level.
  2. For each part you see the machine steps from your workflow and, per CNC step, the program name (often also the barcode).
  3. Expand a program and select an operation. It is highlighted in the preview, so you can see which operation it is.
  4. Check in the operation's properties which machining principle was assigned. A principle name should always be shown there.
  5. If there is no principle, you get a message. Fix that part first.

Common operation terms in the report: CUT (sawing), MILL (milling), DRILL (drilling), RABBET (rebate), GROOVE (groove) and POCKET (pocketing).

Finding the part with the error

The log file shows the internal part numbers as imos knows them. In a large drawing you want to find that part quickly.

  1. In the imos options, enable display of the internal imos ID (PXM) in the imos Manager.
  2. Restart imos.
  3. Look up the number from the log using the imos filter function (by ID).
  4. Regenerate the CNC program for that part only, with the log file, to analyse the error in isolation.

Fixing 'no machining principle found'

Work through the chain from top to bottom. An operation that isn't allowed at the top level will never get a principle.

  1. Machine: check under Possible operations of the correct machine and field that this operation type is assigned.
  2. Workflow: check that the operation types in the workflow step are linked to the machine definition. If not, the operation must be entered there as well.
  3. Right workflow: generate with Automatic, or deliberately pick the intended workflow.
  4. Principle conditions: compare the drawn diameter and depth with the minimum and maximum values in the principle.
  5. Formatting class: check that the material's class matches the class in the principle's conditions.
  6. Operation type: check that the operation as imos sees it (for example POCKET rather than MILL) matches the type in your principle.
  7. Tool: 'Tooldiameter is bigger than the hole' means the cutter in the principle is larger than the drawn feature. Choose a tool that fits.

A real-world example: a pocket got no principle. The only pocketing principle was limited to 27 mm depth, while the drawn pocket was deeper. A longer cutter was available, and an extra principle for that cutter cleared the message.

Tip

With 'unassigned operation', the machine or workflow allows the operation on no position at all. Start with steps 1 and 2. With 'no machining principle found', the cause is usually in steps 4 to 6.

More or fewer programs than expected

  • Through hole drilled from the 'wrong' side: usually correct. imos creates a single program when the through hole can be drilled from the other side.
  • End-face holes split over two programs: if horizontal drilling is only allowed on one end face, imos automatically creates a second program with the part rotated 180 degrees about the Y axis.

Why this approach?

An error message isn't a software fault; it's an analysis that helps you deliver a correct program. Dismiss it, and the software can't assign the right tool, so the operator only finds the problem at the machine. Our rule is simple: an order is only ready for production when there are no error messages. Also aim for error-free reports. If messages keep appearing for parts that are deliberately not allowed on a machine, designers get used to warnings and miss the real error.

Only enable the log file for analysis. Without it, imos generates faster and error messages still appear. When you get one, regenerate that part with the log file.

Frequently asked questions

Should the log file always be on?

No. Only enable it for analysis. Generation is faster without it, and error messages are shown anyway.

Why can't I see the part number from the log in the imos Manager?

The internal imos ID isn't shown by default. Enable it in the imos options and restart imos.

Is the report available in other languages?

In the versions we worked with, the report was in English only. With the list of operation terms (CUT, MILL, DRILL, RABBET, GROOVE, POCKET) it reads quickly.

Some parts can't go on every machine. Is that an error?

Not necessarily. If a part is deliberately not allowed on a machine, route it to the right machine with workflow conditions so the report stays error-free.

Further reading

More than one solution

Almost every question in this knowledge base has more than one solution. The best fit depends on your workflow, machinery and integrations. Not sure which applies to you, or are you using software we don't (yet) support? Feel free to email Wood Intelligence. We're happy to think along with any challenge.

imos is a trademark of imos AG. Wood Intelligence is an independent consultancy.

Download access

Sign in to check whether this download is available.