What Is H-Length? - CNC Zone
594,124 members Register Log in My CNCzone Login Remember Me?
- Advanced Search
- CNCzone®
- Forum
- CAM Software
- SolidCAM for SolidWorks and SolidCAM for Inventor
- What is H-Length?
-
Thread Tools
- Show Printable Version
- Email this Page…
- Subscribe to this Thread…
- Display all images
-
Search Thread
- Advanced Search
- 06-25-2011, 12:32 AM #1 viroy
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
What is H-Length?
Hello, While entering the tool length info in solidcam, there is a field for 'H-Length'. The endmills I have did not come with any information on the H-length value, solidcam defaults to 100, so I left it alone. Anybody know what this is and its importance? Thanks, JSimilar Threads:
Reply with Quote- Tube cut to length
- Fix arc length
- Need Help!- cabie length
- cut to length
- Probe dia and length
- 06-25-2011, 04:36 AM #2 jeffrey001
- View Profile
- View Forum Posts
- View Gallery Uploads
Normally, H goes with a G43 in the Gcode. You should see: T02 M6 G43 H2 If there is no G43, H will have no effect.. H is the offset lenght of the tool Jeff
Reply with Quote - 06-25-2011, 09:47 AM #3 glovebox20
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
Originally Posted by jeffrey001 Normally, H goes with a G43 in the Gcode. You should see: T02 M6 G43 H2 If there is no G43, H will have no effect.. H is the offset lenght of the tool Jeff What jeff is referring to is the tool length offset command for CNC programing. G43 is the G-code to turn on the Tool length offset on most G-code machines (ex. Haas, Fanuc). The H number is the offset you want to use. When setup the tool at the CNC, Most Setup will use the same H# as Tool# to assign the tool length offset value on mills, but dose not have to match. Mill ex: T1 M6 (Change tool, 1/2 EM) G0 G54 G0 X.313 Y.313 S2400 M3 (position table, turn spindle on) G43 H1 Z1. M8 (This line will bring the tool 1. above the apart using tool offset #1) D is typical used for Tool Dia offset along with G41 (Left) or G42 (Right) Z.05 G1 Z-.25 F15. G41 D1 X-.01 Y0 F25. (Cutter Comp on) X1.0 Y-1.0 X0.0 Y.01 G40 X-.313 Y.313 (Cutter Comp off) G0 Z1. M9 G91 G28 G0 Z0 M5 (Bring Z axis to Home Position, Spindle off) M30 I just milled a 1" square, with part Zero being the upper left corner of the part. glovebox20
Reply with Quote - 06-26-2011, 05:08 AM #4 Brakeman Bob
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
Where H Length comes into play is when the user has set up Machine Simulation (or MachSim), especially in five axis machining. The value in H Length is the distance from the tool tip to the gauge line - if you have holders defined and are using them and you have specified the amount the tool projects from the holder in the topography page, H Length will show the combined value. Note that that this made up of the tool, the holder length and the toolholder flange (which is defined in a separate tab in holder definition). It takes a lot of work to set up but I wouldn't be without it.
Reply with Quote - 06-28-2011, 07:42 AM #5 viroy
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
So is that only used during automatic tool change functions? I am not sure what the 'gauge line' is, I'm guessing it's where the collet holds the end-mill (such as a groove for it to lock on to).
Reply with Quote - 06-28-2011, 08:10 AM #6 jeffrey001
- View Profile
- View Forum Posts
- View Gallery Uploads
This is a small pic of where the gauge line is and what is tool length
Attached Thumbnails Reply with Quote - 06-29-2011, 04:05 AM #7 Brakeman Bob
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
Originally Posted by viroy So is that only used during automatic tool change functions? I am not sure what the 'gauge line' is, I'm guessing it's where the collet holds the end-mill (such as a groove for it to lock on to). No, it is nothing to do with automatic tool change but a lot to do with tool offset setting eg G43 calls. The Gauge Line is normally the spindle nose face and is the place where all tool length offsets are measured from (as shown in Jeffs's diagram). If you run your machines with the tool lengths defined in the program, H Length is variable that you would need to set (either manually or automatically) to output the necessary code (presuming that your post is set up to do that.
Reply with Quote - 07-01-2011, 05:29 AM #8 jake_tb
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
We have an old milling machine with an indexing head that rotates 360 degrees around the "Y" axis. The controller is an old Heidenhain TNC 355 that only has one coordinate system and does not have any coordinate transformation/rotation functionality like the "cycle 19" on new Heidenhain controllers. We use the "H" length to allow tricky plane tilting. We have set-up our post processor to use the "H" length as the head pivot to tool tip length. We measure this length for all our tools we want to use, then manually load these values into the tool table in solidcam under the "H" length. This allows SolidCam to calculate the new X, Y, Z positions and generate the code to come out correct for each tool length based on the head rotation angle. It is a bit time consuming to set-up but it allows the machine to do things it would not normally be capable of! Jake T-B
Reply with Quote - 07-04-2011, 06:04 AM #9 viroy
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
Wow seems pretty complex... how do I calculate H-length? Say I would like to get a value for my 10mm 4FL EM, 60mm OAL, 40mm Tool length, 25mm shoulder.
Reply with Quote - 07-05-2011, 04:03 AM #10 Brakeman Bob
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
It's not complex, but it is labour intensive if you want SolidCAM to calculate H-Length automatically. Basically, H-Length is the length of the toolholder sticking out of the spindle nose plus the length of the tool sticking out of the holder, nothing more. To set H-Length manually just tick the check box to the left of the H-Length value box and you can put whatever value you like in there. For SolidCAM to calculate it automatically you need to define (a) the toolholder flange adaption (MAS-BT, DIN, CAT, ANSI etc.) in Tool Holders (the upper box) and (b) the holder itself in the lower box. Then you have set the holder for all the tools in use. Oh, and you also have to set the flange adaption in the MAC file. As I said, it's a lot of work and unless you are using MachSim, it is a lot of work for little reward. I have machines here that have never been set up to use H-Length in posted G code - we set that on the machine via the tool offset table. If you need to set tool offsets via the CNC program then just set H-Length manually. To answer the question you posed about your Ø10 4fl endmill, you are missing two pieces of crucial information. What toolholder are proposing to use and how much is the tool sticking out of the holder?
Reply with Quote - 07-05-2011, 10:28 AM #11 Aussie_CNC
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
Only if you have access to Machine Simulation (the tab in your simulation dialog box) or your post processor uses this value to calculate positioning for 5 Axis head/head machines, should you care about the H-Length value - it does nothing for you otherwise!
Reply with Quote - 07-05-2011, 10:33 PM #12 viroy
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
I do have a rotary axis I plan on using before not too long. I have to disconnect my X axis controller and plug into the rotary, so the rotary becomes my X axis. I have yet to try it out, I have not had time to get into it yet but really look forward to it. I'd like to make a few pool cues later this year. Would I need H-length for rotary operations?
Reply with Quote - 07-05-2011, 11:13 PM #13 Aussie_CNC
- View Profile
- View Forum Posts
- Private Message
- View Gallery Uploads
No, H-Length isn't required for rotary operations unless you were using Machine Simulation or your post processor was setup to do something funky!
Reply with Quote
- Site Areas
- Settings
- Private Messages
- Subscriptions
- Who's Online
- Search Forums
- Forums Home
- Forums
- CNCzone.com Policies / FAQ
- CNCzone's Community Policies
- CNCzone.com FAQ
- Events, Product Announcements Etc
- News Announcements
- Trade Shows / Webinars / Other Events
- Polls
- Videos
- Want To Buy...Need help!
- For Sale Only
- Community Club House
- International / Regional Forums
- Australia, New Zealand Club House
- Brazilian Club House
- Canadian Club House
- European Club House
- French
- German
- Italian
- Norwegian
- Spanish
- United Kingdom
- Mexican Club House
- South Africa Club House
- USA Club House
- Mentors & Apprentice Locator
- Education - Teachers and Students Hangout
- Complaints and Praise Discussions
- Environmental / Alternate Energy
- Computer Technology
- USB, RS232, PARALLEL etc
- Computers / Desktops / Networking
- International / Regional Forums
- Employment Opportunity / RFQ (Request for Quote).
- Manufacture Company Listing
- Employment Opportunity
- RFQ (Request for Quote)
- North America RFQ's
- EUROPE RFQ's
- RFQ Feedback
- Machinery Manual, Brochure / Photo Archives
- Machinery Manuals / Brochures
- Member / Shop Photos
- CAM Software
- Uncategorised CAM Discussion
- ArtCam Pro
- Alphacam
- Autodesk CAM
- Autodesk Post Processors
- BobCad-Cam
- BobCAM for SolidWorks™
- BobCad Post Processors
- Tutorials
- CamWorks
- CamBam
- CutLeader
- Dolphin CAD/CAM
- EdgeCam
- Esprit
- EnRoute
- EZ-CAM Solutions
- FeatureCAM CAD/CAM
- GibbsCAM
- Hypermill
- Mastercam
- Post Processors for MC
- MadCAM
- OneCNC
- PTC Pro/Manufacture
- PowerMILL
- Postprocessor for CAM
- Rhinocam
- SprutCAM
- SheetCam
- Post Processor Files
- Surfcam
- SolidCAM for SolidWorks and SolidCAM for Inventor
- UG NX
- Visual Mill
- Vectric
- Aspire
- Cut2D / Cut3D
- PhotoVCarve and VCarve Pro
- Post Processors
- ZW3D CAM
- CAD Software
- Uncategorised CAD Discussion
- Autodesk
- Logic Trace CNC/DXF
- Rhino 3D
- Solidworks
- ViaCad / Shark
- Mechanical Engineering
- Epoxy Granite
- Linear and Rotary Motion
- Mechanical Calculations/Engineering Design
- T-Slot CNC building
- WoodWorking
- WoodWorking Topics
- WoodWorking Machines
- Uncategorised WoodWorking Machines
- CNC Machining Centers
- Commercial CNC Wood Routers
- Biesse
- Blue Elephant CNC
- Blue Elephant Hot Products
- Camaster
- Chinese Machines
- DynaCNC
- Excitech routers
- Gerber
- Gorilla CNC Machines
- K2CNC
- Larken
- Multicam Machines
- Omni CNC
- Roctech CNC Routers
- Shopsabre
- Stepcraft
- Techno CNC
- XYZ Gantry Routers
- DIY CNC Router Table Machines
- FAQ of DIY CNC Machine Building
- Avid CNC
- CNC Wood Router Project Log
- FineLine Automation
- Joes CNC Model 2006
- Momus Design CNC plans
- Open Source CNC Machine Designs
- Zen Toolworks
- Wood Lathes / Mills
- MetalWorking
- MetalWork Discussion
- Bending, Forging, Extrusion...
- Casting Metals
- Diemaking / Diecutting
- Mass finishing equipment/media/strategies
- Moldmaking
- Welding Brazing Soldering Sealing
- 80/20 TSLOTS / Other Aluminum Framing Systems
- MetalWorking Machines
- Uncategorised MetalWorking Machines
- Vertical Mill, Lathe Project Log
- Bending- and Punching Machines
- Auto Tool Changer
- Drilling- and Milling Machines
- Benchtop Machines
- Taig Mills / Lathes
- X3/SX3/G0619/G0463
- RF-45 Clone Mill
- Mini Lathe
- Turning Machines
- Bridgeport Machines
- Bridgeport / Romi Lathes
- Bridgeport / Hardinge Mills
- Cincinnati CNC
- CNC Swiss Screw Machines
- CITIZEN Machines
- Colchester Tornado lathes
- CNC "do-it-yourself"
- Daewoo/Doosan
- CNC Machining Centres
- Deckel, Maho, Aciera, Abene Mills
- Dyna Mechtronics
- EMCO CNC Machines
- EMCO Lathe
- EMCO Mills
- Fadal
- Haas Machines
- Haas Lathes
- Haas Mills
- Haas Visual Quick Code
- Hardinge Lathes
- Harrison Alpha
- Hitachi Seikis
- HURCO
- Hyundai Kia
- Kitamura
- Knee Vertical Mills
- Mikinimech
- Milltronics
- Mori Seiki Machines
- Mori Seiki lathes
- Mori Seiki Mills
- Novakon
- OKK
- Okuma
- Sharp CNC
- Shopmaster/Shoptask
- Smithy
- South Bend Machinery
- Syil Products
- Tormach Personal CNC Mill
- Tormach Slant Lathe
- Tormach PathPilot™
- Toyoda
- Tree
- Uncategorised MetalWorking Machines
- Manufacturing Processes
- Milling
- Turning
- Drilling
- Grinding
- Chucking and Measuring
- Other Manufacturing Processes
- Safety Zone
- CNC Plasma, EDM / Waterjet Machines
- Waterjet General Topics
- CNC Plasma / Oxy Fuel Cutting Machines
- EDM Discussion General Topics
- Plasma, EDM / Other similar machine Project Log
- Bulltear Industries
- DynaTorch
- PlasmaCam
- Hypertherm Plasma
- Torchmate
- Laser Engraving and Cutting Machines
- Laser Engraving / Cutting Machine General Topics
- Commercial Laser
- AEON Laser
- BODOR Laser
- BOSS Laser
- G.Weike Laser
- Hurricane Laser
- LOGILASE Laser
- Redsail Laser
- Thunder Laser
- Fiber Laser Cutting Topics
- Laser Control Software
- LaserCut
- Laser Hardware
- Laser CO2 Tubes, Diodes, RF and Power Supplies
- P2X4A
- Power-to-X-for-Applications
- Other Machines
- Other Machine Topics
- CNC Wire Foam Cutter Machines
- Digitizing and Laser Digitizing
- Engraving Machines
- Machine Created Art
- Printing, Scanners, Vinyl cutting and Plotters
- PCB milling
- Commercial Products / Manufacturers Support Forums
- Automation Technology Products
- Bulltear Industries Support Forum
- Charter Oak Automation Support Forum
- CNC4PC
- Maintenance in General
- Maintenance DIY Discussion
- BallScrew Repair
- SERVICE FOR CNC-MACHINES
- Maintenance DIY Discussion
- CNC Electronics
- CNC Machine Related Electronics
- DeskCNC Controller Board
- Dmm Technology
- Gecko Drives
- G-REX
- Hobbycnc (Products)
- Phase Converters
- Leadshine
- PIC Programing / Design
- Rutex Products
- Servo Drives
- Servo Motors / Drives
- SmoothStepper Motion Control
- Stepper Motors / Drives
- Spindles / VFD
- UHU Servo Controllers
- Viper Servo drives
- Xylotex
- Machine Controllers Software and Solutions
- CNC (Mill / Lathe) Control Software (NC)
- Centroid CNC Control Products
- Bosch Rexroth
- CamSoft Products
- Controller Cards
- Controller & Computer Solutions
- Dynapath
- Dynomotion/Kflop/Kanalog
- EdingCNC
- CNC-EDITOR
- CS-Lab CNC Products
- LinuxCNC (formerly EMC2)
- Deckel / Dialog
- FlashCut CNC
- Fagor Automation
- Mori Seiki Software
- Mazak, Mitsubishi, Mazatrol
- Fanuc
- G-Code Programing
- Parametric Programing
- Mach Software (ArtSoft software)
- Mach Wizards, Macros, & Addons
- Machines running Mach Software
- Mach Lathe
- Mach Mill
- Mach Plasma / Laser
- Mach 4
- Screen Layouts, Post Processors & Misc
- Fidia
- DNC Problems and Solutions
- Mitsubishi controls
- NCPlot G-Code editor / backplotter
- SIEMENS Sinumerik CNC controls
- SIEMENS -> GENERAL
- SIEMENS -> Sinumerik 802D/808D/810D/828D/840D
- SIEMENS -> Sinumerik 810M/810T
- SIEMENS -> Sinumerik 840C
- SIEMENS -> ShopMill
- SIEMENS -> ShopTurn
- SIEMENS -> SinuTrain
- UCCNC Control Software
- PlanetCNC
- HEIDENHAIN
- HEIDENHAIN -> GENERIC
- HEIDENHAIN -> MillPlus
- HEIDENHAIN -> iTNC530 PC-SOFTWARE
- HEIDENHAIN -> ManualPlus / CNC Pilot
- HEIDENHAIN -> TNC
- Index and Traub
- Visual Basic
- WinCnc
- Okuma
- Philips
- OpenSource CNC Design Center
- Opensource Forum Rules
- Arduino
- Coding
- OpenSource Software
- Open Source Controller Boards
- Engraving / Art Design Software
- Jewelry Design Software
- SignMaking
- Signmaking Topics
- Portfolio Board
- Additive Manufacturing / 3D Printers and 3D Scanners
- 3D Printer / 3D Scanner Discussion
- 3D Printing / Scanning Software and Hardware
- Electronics
- Material Technology
- Material Machining Solutions
- Composites, Exotic Metals etc
- Glass, Plastic and Stone
- Vacuum forming, Thermoforming etc
- Metallurgy
- Plastic injection
- Hard / High Speed Machining
- Tools / Tooling Technology
- Calibration / Measurement
- CNC Tooling
- Metalworking- / Woodworking Tooling / Manual Machining
- Work Fixtures / Hold-Down Solutions
- Toolgrinding / Toolgrinding Machines
- Hobby Projects
- Hobby Discussion
- Wooden Clocks
- Gunsmithing
- I.C. Engines
- Musical Instrument Design and Construction
- RC Robotics and Autonomous Robots
- CNCzone®
- Forum
- CAM Software
- SolidCAM for SolidWorks and SolidCAM for Inventor
- What is H-Length?
Tags for this Thread
its, notView Tag Cloud
Posting Permissions
- You may not post new threads
- You may not post replies
- You may not post attachments
- You may not edit your posts
- BB code is On
- Smilies are On
- [IMG] code is On
- [VIDEO] code is On
- HTML code is Off
Forum Rules
-- Default Style -- Default MobileAbout CNCzone.com
- We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!
Quick Links
- My User CP
- Advertising Rates
- Site Support
- Imprint
Follow us on
All times are GMT -4. The time now is 01:23 PM. All CNCzone.com Content - Copyright © 2019 - All Rights Reserved CNC Machines,CAD/CAM,Milling Machines,Lathes,Classifieds, Lasers,Engraving,woodworking,MetalWorking,Industrial Equipment, Manufacturing technolgies
Our Brands
Từ khóa » G43 H1 G Code
-
What Is Tool Length Compensation In Cnc? - G43, G44 Etc
-
Tool Length - G43 - Expert CNC
-
CNC Mill Program G91 G41 G43
-
G Codes - LinuxCNC
-
Explaination Of G43, And G44 Please | Practical Machinist
-
G-Code G43 Z## H## Not Working On My CNC Mill And Auto-add ...
-
Tool Offsets - Dlsweb..au
-
Unit 4: CNC Language And Structure – Manufacturing Processes 4-5
-
Tool And Radius Offsets (G40–G49) - WinMax Help Center
-
G Code G43, CNC Coding Guide
-
G41 And G42 Cutter Compensation - G-Code Tutor
-
[PDF] G & M Code REFERENCE MANUAL - MachMotion
-
G43 Tool Length Compensation + (Add) / G44 Tool Length Comp...