After a run, Machinability feedback in the Program stage lists holes CAM Assist couldn't make with a hole-making operation, and why. Usually the cause is a missing tool or a setup that can't reach the hole. This article walks through the common causes.
Which issue do you see?
In the Program stage, click Machinability feedback to see the list.
| Issue | Meaning |
|---|---|
| Hole unmachinable | No tool in your selected libraries could make the hole with a hole-making operation. |
| Hole cannot be drilled | No drill could be used. Another process may still make the hole. |
| Spot drilling unavailable | The hole is drilled without a spot drill. |
| Hole cannot be reamed | No reamer could be used. Another process may still finish the bore. |
| Hole cannot be bored with an end mill | Helical boring with an end mill couldn't be used. |
| Thread cannot be machined | No tap or thread mill could cut the thread. |
| Thread may be incomplete | The thread can be cut, but less deep than requested. |
| Hole chamfer cannot be machined | No tool could cut the chamfer. |
| Plain-hole machining issue | Some plain holes can't be machined fully; others use a different process. |
Click the issue to see each cause, its recommended change, and whether it stops CAM Assist machining those holes or only affects the result. Before a run, the Assessment stage may show Hole requires boring with an end mill: CAM Assist will try other operation types for those holes.
Does a hole group say "Needs attention"?
The Feature planning stage groups the part's holes. Its status banner shows "1 hole group has machinability issues." (or the number of groups), and each affected card is marked Needs attention. The card lists the problem, for example:
- "The hole has undercuts."
- "The hole shape is not fully defined, or contains a shape CAM Assist cannot machine, such as a fillet."
- "The hole shape is not supported."
- "The hole cannot be machined because it has no entry from a perpendicular surface."
- "Thread depth too shallow. Depth must be at least one pitch."
For a thread that's too shallow, change the Thread depth. See Hole element settings. For a shape CAM Assist can't make, click Don't machine on the card, then choose Machined as geometry to rough and wall-finish it like a pocket, or Excluded from program to leave it unmachined for you to program yourself. See Review and edit hole groups in Feature planning.
If the banner says "Hole planning couldn't run for this part.", click Try again in the stage. See "Couldn't finish assessing machinability".
Is a suitable tool missing?
Messages like "CAM Assist could not find a usable tap for this thread." or "CAM Assist could not find a usable drill for this hole." mean no tool in your selected libraries fits.
- In the Tools stage, check your chosen libraries for the tool the message names, with the right diameter, length, and for taps and thread mills the right thread form and pitch. CAM Assist works out the tap drill (core hole) size from the tap's thread; you can't set it yourself. See Add or remove tool libraries for a part.
- Make sure the tool is allowed for the stock material and has cutting data for it. See Set a tool's allowed usages.
- Click Run CAM Assist again.
Can the setup reach the hole?
| Message | What to do |
|---|---|
| "CAM Assist could not machine this hole from any of the enabled setups." | Include more setups in the Setups stage. See Set up your setups. If you limited the hole group to certain setups in Feature planning, CAM Assist only machines it in those: add a setup that can reach the hole under Restrict to setups, or drag the card back to Any setup. See Choose which setups machine a group. |
| "The machine cannot orient the tool to reach this hole from this setup." | Choose a different Mode for the setup. See Machining modes. |
| "CAM Assist could not machine this hole because it requires a machining direction that was not specified by the user." | Add the hole's axis direction to the setup's machining directions. See Choose machining directions for 3+2. |
| "CAM Assist tried to machine the hole from a setup where the hole is obstructed." | Check the model and the geometry around the hole. |
| "No suitable tool can safely access the hole due to collisions with the part." | Check the tools and the geometry around the hole. |
| "CAM Assist could not determine a machining direction for this hole." | The hole may be misaligned. Check the modeled hole. |
Is the thread too deep or too shallow?
- "Available tools cannot cut a complete thread at least one pitch deep.": check the hole is deep enough for the thread.
- "The selected threading operation will produce less thread depth than requested.": there isn't enough room at the bottom of the hole for the full thread. Change the Thread depth or the hole if that matters. See Hole element settings.
Still not working?
If you've checked all of the above, contact CloudNC support. Include the part file, your tool library and your CAM Assist log files: see Find your CAM Assist log files.