Tool Properties - Customer Guide

Overview

The Tool Properties Tab is where you configure the specifications for each CNC tool in your library. Mozaik includes sample tools, but all specifications must be verified and adjusted for your specific machine and shop requirements before generating G-Code.

CRITICAL: Always verify tool properties match your actual tooling and CNC machine capabilities.

Tool Parameters

1. Tool Image

Add a JPG image of the tool for visual reference.

How to add:

• Click the space below "Tool Parameters"
• Browse to your image file
• Images are stored in: C:\Mozaik\Data\CNC\Images

Purpose: Visual aid to quickly identify tools. Not used in G-Code generation.

2. Tool Diameter

Enter the exact cutting diameter of your tool.

CRITICAL: Must be accurate for proper toolpath calculation.

Important notes:

• Measure actual diameter, don't rely on nominal size
• If you sharpen tools, update diameter after sharpening
• Worn or re-sharpened bits have smaller diameters
• Incorrect diameter causes incorrect part sizing

Example: A 3/8" bit worn to 0.37" should be entered as 0.37"

3. Pass Depth

Maximum depth the tool should cut in a single pass.

Guidelines:

• Must be less than tool's cutting edge length
• Deeper passes = faster cutting but more tool wear
• Shallower passes = slower but cleaner cuts

How it works:

• Material: 1" thick
• Pass Depth: 3/4"
• Result: Two passes (3/4" + 1/4")

Typical values:

• Roughing: 1/2" to 3/4"
• Finishing: 1/4" to 3/8"
• Hard materials: Reduce by 25-50%

Note: Pass depth is added to small part handling settings.

4. Tool Type

Select the bit type from dropdown.

Common types:

• Compression
• Downshear
• Upshear
• Straight
• V-Bit
• Profile bits
• Panel raising bits

Why it matters: Affects chip evacuation, surface finish, and appropriate applications.

Advanced Parameters

5. Stepover

Distance between toolpath centerlines when pocketing or machining dados.

What it is: Horizontal spacing between passes

Guidelines:

• Typical: 40-60% of tool diameter
• Roughing: 50-60% (faster, rougher finish)
• Finishing: 30-40% (slower, smoother finish)

Example:

• Tool diameter: 3/8" (0.375")
• Stepover 50%: 0.1875"
• Each pass overlaps previous by 50%

Visual: Imagine a tool making parallel passes - stepover is the distance between each pass centerline.

6. Plunge Depth

Maximum depth the tool can plunge straight down into material.

Purpose: Controls vertical entry depth

Guidelines:

• Usually equal to or less than pass depth
• Aggressive plunge can break small tools
• Conservative plunge extends tool life

Typical: Same value as Pass Depth

7. Add for Thru Cut

Extra depth added when cutting completely through material.

Purpose: Prevents chipping on bottom surface by ensuring complete cut-through.

Recommended: 0.005" to 0.015" (0.1mm to 0.4mm)

How it works:

• Material: 0.75" thick
• Add for Thru Cut: 0.010"
• Actual cut depth: 0.760" (cuts into spoilboard slightly)

Why needed: Ensures clean bottom edge without tearout.

8. Pocket Ramp

Horizontal distance tool travels when ramping into a pocket.

What it is: Gradual angled entry instead of plunging straight down

Benefits:

• Reduces tool wear
• Smoother cutting action
• Better for smaller tools

Value guidance:

• 0 = No ramp (plunge straight down)
• 1" = Gentle 1" horizontal ramp
• Typical: 0.5" to 2"

NOTE: Only applies to pocket toolpaths, NOT dados or grooves.

Tool Specifications

9. Tool Spec PDF

Attach manufacturer specification documents to tools.

How to add:

1. Save spec document with EXACT same name as tool
2. Formats: .pdf, .jpg, or .doc
3. Place in: C:\Mozaik\Data\CNC\ToolSpecs
4. Click "Tool Specs" button to view

Example:

• Tool name: "RoyceAyr R68-02002"
• Spec file: "RoyceAyr R68-02002.pdf"

Use for: Quick reference to manufacturer specs, cutting parameters, and diagrams.

Feeds and Speeds

10. Feeds and Speeds

Configure spindle speed, feed rate, and plunge rate.

How Min/Max works:

• Set Min and Max values
• Material Library has cutting % (0-100%)
• Mozaik calculates: Actual = Min + (Max - Min) × Material%

For constant speed:

• Set Min = Max
• Set Material Library to 100%

Parameters:

Spindle Speed (RPM):

• Rotation speed of spindle
• Typical: 16,000 - 18,000 RPM
• Higher for smaller bits
• Lower for larger bits

Feed Rate (In/Min or mm/Min):

• How fast tool moves through material
• Typical: 300-500 In/Min
• Faster = quicker cuts, more tool wear
• Slower = cleaner finish, longer tool life

Plunge Rate (In/Min or mm/Min):

• How fast tool plunges vertically
• Always slower than feed rate
• Typical: 50-100 In/Min
• Too fast can break small tools

Example:

Spindle: 16000 to 18000 RPM
Feed: 400 to 400 In/Min (constant)
Plunge: 60 to 70 In/Min

Tool Applications

11. Roughing Tool Type

Designate tool for roughing operations.

☑ Roughing

What roughing does:

• Removes bulk material quickly before final cutout
• Uses less expensive bit for heavy cutting
• Saves wear on finishing cutout tool

When roughing is used:

1. Part has a "skin" (Full Sheet, Onion Skin, or Return Skinning)
2. Roughing tool is in the active Toolset

Skinning types:

• Full Sheet Skin: Leave skin on all parts
• Onion Skin: Multiple roughing passes
• Return Skin: Roughing for re-entry cuts

Configure in: Cutout Options menu

Note: If multiple Roughing tools in toolset, first one is used.

12. Tool Application

Define what operations this tool performs.

13. Sharp Corner

Enable sharp corner toolpaths with V-bits.

☑ Sharp Corners

What it does:

• Automatically adds corner-sharpening toolpath
• Uses V-bit to create true 90° corners
• Necessary for square corners in pockets

V-bit selection: Based on included angle:

• 22.5°
• 30°
• 45°
• 60°
• 90°
• 110°
• 120°
• 140°

IMPORTANT: Mozaik uses the INCLUDED ANGLE (total angle of V), not half-angle.

Use in: Panel Tool Groups for doors with sharp corners

14. CNC Door

Enable and define profile tools for door work.

☑ CNC Door

When checked:

• "Shape Tool" button appears
• Opens Tool Shape Editor
• Draw cross-section of tool profile

How to use:

1. Check "CNC Door"
2. Click "Shape Tool"
3. Add points to define profile
4. Move and shape points to match tool
5. Save profile

Pre-configured tools: Mozaik includes many standard door tools from manufacturers. Custom or specialized tools need to be drawn manually.

Use for:

• Panel raising bits
• Edge profile bits
• Ogee, cove, bead profiles
• Any router bit with a profile

Additional Settings

15. Priority

Control machining order for manually added toolpaths only.

When used: ONLY for custom user-added toolpaths

How it works:

• Lower number = runs first
• Higher number = runs later
• Default Mozaik operations ignore this

Typical use: Ensuring custom operations run in specific sequence.

16. Mapping Number (Map T#)

Tool number mapping for specific post-processors.

Required for:

• Homag/Weeke Woodwop
• Felder machines
• SCM Maestro
• HolzHer
• Other custom post-processors

How to use:

1. Click on tool
2. Enter machine's tool number in "Map T#"
3. Matches Mozaik tool to machine's tool numbering

Note: Only needed for specific CNC controllers. Standard post-processors don't require mapping.

You don't need to map all tools - only the tools you actually use.

Tool Management

17. Sidebar Buttons

Manage tools in your library:

18. Tooling Spreadsheet

View and edit all tools in grid format.

How to access: Click "Tooling Spreadsheet" button

Features:

• See all tools and properties at once
• Edit values directly in grid
• Print complete tool library
• Export/import multiple tools
• Quick comparison of settings

Benefits:

• Easier than editing one tool at a time
• Good for batch updates
• Print for shop reference
• Verify consistency across similar tools

Creating a New Tool

Step-by-Step:

1. Click "Add Tool"
2. Name the tool (Example: "3/8 Compression Spiral")
3. Add tool image (optional but recommended)
4. Enter Tool Parameters:
   • Diameter: (exact measurement)
   • Pass Depth: (maximum per pass)
   • Tool Type: (from dropdown)
5. Configure Advanced Parameters:
   • Stepover: (40-60% of diameter)
   • Plunge Depth: (usually = pass depth)
   • Add for Thru Cut: (0.010")
   • Pocket Ramp: (0.5" to 2")
6. Set Feeds and Speeds:
   • Spindle Speed: Min and Max RPM
   • Feed Rate: Min and Max In/Min
   • Plunge Rate: Min and Max In/Min
7. Assign Tool Application:
   • Check appropriate box (Cutout, Drill, Dado, etc.)
8. Special configurations:
   • Sharp Corners: If V-bit
   • CNC Door: If profile tool
   • Roughing: If roughing bit
9. Save (click OK)

Tips for Success

💡 Verify before G-Code - Always check tool specs match your actual tools

💡 Update after sharpening - Sharpened tools have smaller diameters

💡 Start conservative - Use slower feeds/speeds, then optimize

💡 Document your settings - Keep notes on what works well

💡 Use Tool Spec PDFs - Attach manufacturer specs for reference

💡 Copy similar tools - Duplicate and modify rather than starting from scratch

💡 Test on scrap - Verify new tool settings on scrap before production

💡 Check pass depth - Never exceed tool's cutting edge length

💡 Stepover affects finish - Lower stepover = smoother but slower

💡 Export for backup - Save custom tools in case of reinstall

Frequently Asked Questions

Q: Why must I verify Mozaik's sample tools?
A: Sample tools are generic examples. Your actual tools may have different specs, and your CNC may have different capabilities.

Q: What happens if tool diameter is wrong?
A: Parts will be wrong size. Too large = part too small. Too small = part too large. Always measure actual diameter.

Q: How do I know what feeds and speeds to use?
A: Start with manufacturer recommendations, then adjust based on results. Too fast = rough finish or broken tools. Too slow = burn marks or excess wear.

Q: Why use Min and Max for feeds/speeds?
A: Allows automatic adjustment based on material. Hard materials use slower speeds (closer to Min), soft materials can go faster (closer to Max).

Q: What's the difference between Feed Rate and Plunge Rate?
A: Feed Rate is horizontal movement speed. Plunge Rate is vertical (downward) speed. Plunge Rate should always be slower.

Q: Do I need Sharp Corners checked for all tools?
A: No, only for V-bits used to create sharp 90° corners in pockets. Standard bits don't need this.

Q: What if I don't have manufacturer specs?
A: Measure the tool carefully, start with conservative settings, and test on scrap. Adjust based on results.

Q: Can I use the same tool for roughing and finish cutting?
A: Yes, but it's better to have a dedicated roughing tool to save wear on your finish cutout tool.

Q: What's a good starting Feed Rate?
A: Start around 300-400 In/Min for general work. Increase if finish is good and tool handles it well.

Q: Why does my tool break when plunging?
A: Plunge Rate might be too fast, or Plunge Depth too aggressive. Reduce both and try again.