{"id":5120,"date":"2024-02-03T13:00:00","date_gmt":"2024-02-03T12:00:00","guid":{"rendered":"https:\/\/cncgraf.com\/?p=5120"},"modified":"2024-02-04T11:09:26","modified_gmt":"2024-02-04T10:09:26","slug":"g-code-drilling-cycle-g82-cycles-drilling-programme","status":"publish","type":"post","link":"https:\/\/cncgraf.com\/en\/2024\/02\/03\/g-code-bohrzyklus-g82-zyklen-bohrprogramm\/","title":{"rendered":"G-code drilling cycle G81, G82, G83, G73 and G84: Step-by-step instructions"},"content":{"rendered":"<div class=\"wp-block-group alignfull has-base-background-color has-background has-global-padding is-layout-constrained wp-container-core-group-is-layout-4145d225 wp-block-group-is-layout-constrained\" style=\"padding-right:0;padding-left:0\">\n<div style=\"height:30px\" aria-hidden=\"true\" class=\"wp-block-spacer\"><\/div>\n\n\n\n<h1 class=\"wp-block-heading alignwide has-text-align-center has-base-background-color has-background has-large-font-size\" id=\"g-code-bohrzyklus-g-81-g-82-g-83-g-73-und-g-84-schritt-fur-schritt-anleitung\">G-code drilling cycle G81, G82, G83, G73 and G84: Step-by-step instructions<\/h1>\n\n\n\n<p class=\"wp-block-paragraph\">In the previous blog posts, \u201e<a href=\"https:\/\/cncgraf.com\/en\/2023\/12\/20\/cnc-programming-g-code-learn-commands\/\" data-type=\"post\" data-id=\"3742\">CNC programming: Learn G-code - Quick and easy<\/a>\u201c and \u201e<a href=\"https:\/\/cncgraf.com\/en\/2024\/01\/15\/cnc-programming-g-code-learning-part2\/\" data-type=\"post\" data-id=\"4387\">Learning G-Code Part 2\/2: Advanced CNC programming<\/a>\u201e, we learnt the basics and advanced aspects of G-code programming. However, one important G-code command has not yet been covered in these articles - the G-code drilling cycle.<br><br>In this article, we will take a detailed look at the G-code drilling cycle. You can then easily integrate these commands into your projects. Have fun reading!<br><br>We use our free G-Code Simulator as a working tool <a href=\"https:\/\/cncgraf.com\/en\/cncgraf-8-cnc-control-software-range-of-functions\/\" data-type=\"page\" data-id=\"8\">cncGraF<\/a>.<br>\u201e<a href=\"https:\/\/cncgraf.com\/en\/download-cncgraf-cnc-control-software\/\" target=\"_blank\" rel=\"noreferrer noopener\">Click here to download cncGraF free of charge\u201c<\/a>.<\/p>\n\n\n\n<p class=\"wp-block-paragraph\">To find out more about our G-Code Simulator, please click here<br>\u201e<a href=\"https:\/\/cncgraf.com\/en\/2023\/12\/20\/free-g-code-simulator-cnc-emulator\/\" data-type=\"post\" data-id=\"3822\">cncGraF: Free G-code simulator and CNC machine emulator<\/a>\u201e.<\/p>\n\n\n\n<figure class=\"wp-block-image size-large is-resized\"><img loading=\"lazy\" decoding=\"async\" width=\"1024\" height=\"836\" src=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-1024x836.jpg\" alt=\"cncGraF 8: Free G-code simulator and CNC machine emulator\" class=\"wp-image-4998\" style=\"width:625px;height:auto\" srcset=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-1024x836.jpg 1024w, https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-600x490.jpg 600w, https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-300x245.jpg 300w, https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-768x627.jpg 768w, https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei-15x12.jpg 15w, https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/12\/g-code-teil2-datei-komplette-g-code-datei.jpg 1045w\" sizes=\"auto, (max-width: 1024px) 100vw, 1024px\" \/><\/figure>\n\n\n\n<div class=\"wp-block-rank-math-toc-block\" id=\"rank-math-toc\"><h4>Overview<\/h4><nav><ul><li class=\"\"><a href=\"#bohren-ohne-g-code-bohrzyklus\">Drilling without G-code Drilling cycle<\/a><\/li><li class=\"\"><a href=\"#g-code-bohrzyklus-g-81-und-g-82\">G-code drilling cycle: G81 and G82<\/a><\/li><li class=\"\"><a href=\"#g-code-befehl-g-80\">G-Code command: G80<\/a><\/li><li class=\"\"><a href=\"#g-code-bohrzyklus-g-83-tieflochbohren-mit-spanabfuhr\">G-code drilling cycle: G83 Deep-hole drilling with chip removal<\/a><\/li><li class=\"\"><a href=\"#g-code-bohrzyklus-g-73-tieflochbohren\">G-code drilling cycle: G73 Deep hole drilling<\/a><\/li><li class=\"\"><a href=\"#g-code-gewindebohrzyklus-g-84\">G-code tapping cycle: G84<\/a><\/li><\/ul><\/nav><\/div>\n\n\n\n<div style=\"height:20px\" aria-hidden=\"true\" class=\"wp-block-spacer\"><\/div>\n\n\n\n<hr class=\"wp-block-separator alignfull has-text-color has-tertiary-color has-alpha-channel-opacity has-tertiary-background-color has-background\"\/>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-global-padding is-layout-constrained wp-container-core-group-is-layout-4145d225 wp-block-group-is-layout-constrained\" style=\"padding-right:0;padding-left:0\">\n<h2 class=\"wp-block-heading has-base-background-color has-background has-large-font-size\" id=\"bohren-ohne-g-code-bohrzyklus\">Drilling without G-code Drilling cycle<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">As drilling only requires a lowering in the Z-axis, this can also be carried out without the G-code drilling cycle. To do this, simply use the G-code command <strong>G01 Z<\/strong> is used. An example (excerpt) of the corresponding G-code looks like this:<\/p>\n\n\n\n<figure class=\"wp-block-table is-style-stripes\"><table><thead><tr><th class=\"has-text-align-left\" data-align=\"left\">Example <\/th><\/tr><\/thead><tbody><tr><td class=\"has-text-align-left\" data-align=\"left\"><em>; 10 mm into the workpiece at a feed rate of 600 mm per minute<\/em><br><strong>G01 Z-10 F600<\/strong><br><em>; wait 1 second<\/em><br><strong>G04 H1<\/strong><br><em>; Lift the tool at rapid speed to the height Z = 5 mm above the zero point<\/em><br><strong>G00 Z5<\/strong><\/td><\/tr><\/tbody><\/table><figcaption class=\"wp-element-caption\">Drilling with <strong>G01 Z<\/strong> without G-code drilling cycle<\/figcaption><\/figure>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-global-padding is-layout-constrained wp-block-group-is-layout-constrained\">\n<hr class=\"wp-block-separator alignfull has-text-color has-tertiary-color has-alpha-channel-opacity has-tertiary-background-color has-background\"\/>\n\n\n\n<h2 class=\"wp-block-heading has-base-background-color has-background has-large-font-size\" id=\"g-code-bohrzyklus-g-81-und-g-82\">G-code drilling cycle: G81 and G82<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">The simplest drilling cycle is the G-code command <strong>G81<\/strong>. This drilling cycle is used for simple drilling, while the command <strong>G82 <\/strong>additionally enables drilling with a dwell time at the bottom of the hole.<br><br>The <strong>G81<\/strong>\/<strong>G82<\/strong>-command has the following syntax: <br><strong>G98(G99) G81(G82) X Y Z R F (P)<\/strong><br><br>The parameters are as follows:<\/p>\n\n\n\n<ol class=\"wp-block-list\">\n<li>With the parameter <strong>G98<\/strong>\/<strong>G99 <\/strong>The retraction height to which the tool should move after the drilling cycle is defined.<br><strong>G98 <\/strong>- The starting height (starting height) is approached after the drilling cycle.<br><strong>G99 <\/strong>- the retraction height (defined in the parameter <strong>R<\/strong>) is approached after the drilling cycle.<br><img loading=\"lazy\" decoding=\"async\" width=\"24\" height=\"24\" class=\"wp-image-1775\" style=\"width: 24px;\" src=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/08\/info.png\" alt=\"\"> <strong>Note:<\/strong> If no parameter <strong>G98 <\/strong>or <strong>G99 <\/strong>is specified, then <strong>G98<\/strong>.<\/li>\n\n\n\n<li>The parameters <strong>X,Y,Z<\/strong>: <br><strong>X<\/strong> - Position X<br><strong>Y<\/strong> - Position Y<br><strong>Z<\/strong> - Depth Z (absolute)<\/li>\n\n\n\n<li><strong>R<\/strong> - Incremental value of the retraction plane, in relation to the starting point in the Z-axis<\/li>\n\n\n\n<li><strong>F<\/strong> - Feed speed in mm\/min<\/li>\n\n\n\n<li>The G-Code drilling cycle <strong>G82 <\/strong>also has the parameter <strong>P<\/strong> for waiting time in milliseconds <br>(1000ms = 1sec.) at the bottom of the hole<\/li>\n<\/ol>\n\n\n\n<figure class=\"wp-block-table is-style-stripes\"><table><thead><tr><th class=\"has-text-align-left\" data-align=\"left\">Example<\/th><\/tr><\/thead><tbody><tr><td class=\"has-text-align-left\" data-align=\"left\"><strong>G00 Z0<\/strong><br><strong>G98 G82 X10 Y10 Z-3 F300 P100<\/strong><\/td><\/tr><\/tbody><\/table><figcaption class=\"wp-element-caption\">Drilling cycle <strong>G82<\/strong> with the parameter <strong>P<\/strong><\/figcaption><\/figure>\n\n\n\n<p class=\"wp-block-paragraph\">In the example above, a hole is drilled at positions X10 and Y10, with a drilling depth of 3 millimetres. In addition, a dwell time (parameter <strong>P<\/strong>) of 100 milliseconds, during which the milling machine pauses. At the end of the drilling process, the starting height, which in this case is Z=0, is approached again.<\/p>\n\n\n\n<h2 class=\"wp-block-heading has-base-background-color has-background has-large-font-size\" id=\"g-code-befehl-g-80\">G-Code command: G80<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">The drilling cycle is started with the command <strong>G80<\/strong> or by another G-code command such as <strong>G00 <\/strong>or <strong>G01 <\/strong>deleted.<\/p>\n\n\n\n<figure class=\"wp-block-table is-style-stripes\"><table><thead><tr><th class=\"has-text-align-left\" data-align=\"left\">Example<\/th><\/tr><\/thead><tbody><tr><td class=\"has-text-align-left\" data-align=\"left\"><strong>G98 G82 X20 Y20 Z-3 F300 P100<\/strong><br><em>; Repeat drilling cycle at three points <\/em><br>X30 Y20<br>X40 Y20<br>X50 Y20<br><em>; Delete drilling cycle<\/em><br><strong>G80<\/strong><\/td><\/tr><\/tbody><\/table><figcaption class=\"wp-element-caption\">In this example, the drilling cycle <strong>G82 <\/strong>with the specified parameters. The drilling cycle is then repeated 3 times at different positions, whereby the settings of the drilling cycle are retained. Finally, the drilling cycle is ended with <strong>G80<\/strong> deleted.<\/figcaption><\/figure>\n\n\n\n<hr class=\"wp-block-separator alignfull has-text-color has-tertiary-color has-alpha-channel-opacity has-tertiary-background-color has-background\"\/>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-global-padding is-layout-constrained wp-block-group-is-layout-constrained\">\n<h2 class=\"wp-block-heading has-base-background-color has-background has-large-font-size\" id=\"g-code-bohrzyklus-g-83-tieflochbohren-mit-spanabfuhr\">G-code drilling cycle: G83 Deep-hole drilling with chip removal<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">Compared to the drilling cycles <strong>G81<\/strong>\/<strong>G82<\/strong> this drilling cycle contains an additional parameter <strong>Q<\/strong>. The parameter <strong>Q<\/strong> is used to control the chip removal. As chips are produced during drilling, this drilling cycle is particularly recommended for deep hole drilling.<br><br>The <strong>G83<\/strong>-command has the following syntax: <br><strong>G98(G99) G83 X Y Z R F P Q<\/strong><\/p>\n\n\n\n<p class=\"wp-block-paragraph\">The parameters are the same as for the G-code drilling cycle <strong>G81\/G82<\/strong>, but with an additional parameter:<br><strong>Q<\/strong> - Drilling depth per infeed defined in millimetres<\/p>\n\n\n\n<figure class=\"wp-block-table is-style-stripes\"><table><thead><tr><th class=\"has-text-align-left\" data-align=\"left\">Example<\/th><\/tr><\/thead><tbody><tr><td class=\"has-text-align-left\" data-align=\"left\"><strong>G00 Z0<\/strong><br><strong>G98 G83 X10 Y10 Z-9 F300 P100 Q3<\/strong><\/td><\/tr><\/tbody><\/table><figcaption class=\"wp-element-caption\">Drilling cycle <strong>G83 <\/strong>with the parameter <strong>Q<\/strong><\/figcaption><\/figure>\n\n\n\n<p class=\"wp-block-paragraph\">In the example above, a hole is drilled at positions X10 and Y10, with a drilling depth of 9 millimetres. In addition, a dwell time of 100 milliseconds is executed at the bottom of the hole, during which the milling machine pauses. The hole is drilled with a triple infeed, as the plunge depth per infeed is 3 millimetres (parameter <strong>Q<\/strong>). At the end of the drilling process, the initial height Z=0 is approached. The graphic below explains the parameter <strong>Q<\/strong>.<\/p>\n\n\n\n<figure class=\"wp-block-image size-full\"><img loading=\"lazy\" decoding=\"async\" width=\"481\" height=\"296\" src=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2024\/02\/parameter-q.jpg\" alt=\"The parameter Q: G-code drilling cycle G83 \" class=\"wp-image-5202\" srcset=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2024\/02\/parameter-q.jpg 481w, https:\/\/cncgraf.com\/wp-content\/uploads\/2024\/02\/parameter-q-300x185.jpg 300w, https:\/\/cncgraf.com\/wp-content\/uploads\/2024\/02\/parameter-q-18x12.jpg 18w\" sizes=\"auto, (max-width: 481px) 100vw, 481px\" \/><\/figure>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-global-padding is-layout-constrained wp-block-group-is-layout-constrained\">\n<h2 class=\"wp-block-heading has-base-background-color has-background has-large-font-size\" id=\"g-code-bohrzyklus-g-73-tieflochbohren\">G-code drilling cycle: G73 Deep hole drilling<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">This drilling cycle corresponds to drilling cycle G83, with the difference that a short lift-off distance is approached after each chip removal with Q. The setting for the lift-off distance can be made in cncGraF under \u201eSettings -&gt; Options -&gt; G-Code\u201c.<\/p>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-tertiary-background-color has-background has-global-padding is-layout-constrained wp-block-group-is-layout-constrained\">\n<hr class=\"wp-block-separator alignfull has-text-color has-cyan-bluish-gray-color has-alpha-channel-opacity has-cyan-bluish-gray-background-color has-background\"\/>\n\n\n\n<h2 class=\"wp-block-heading has-tertiary-background-color has-background has-large-font-size\" id=\"g-code-gewindebohrzyklus-g-84\">G-code tapping cycle: G84<\/h2>\n\n\n\n<p class=\"wp-block-paragraph\">Finally, we turn our attention to the supreme discipline of tapping with the G-code command <strong>G84<\/strong>. This command can be used to create both right-hand and left-hand threads. Please note that a spindle with both anti-clockwise and clockwise rotation is required.<\/p>\n\n\n\n<p class=\"wp-block-paragraph\"><img loading=\"lazy\" decoding=\"async\" width=\"24\" height=\"24\" class=\"wp-image-1775\" style=\"width: 24px;\" src=\"https:\/\/cncgraf.com\/wp-content\/uploads\/2023\/08\/info.png\" alt=\"\"> <strong>Note:<\/strong> In cncGraF under \u201eSettings -&gt; Options -&gt; G-Code\u201c, the option \u201e<strong>Use old G84 version<\/strong>\u201c must be deactivated. This old version of the <strong>G84 <\/strong>command does not comply with the G-Code standard, but is still supported by cncGraF to ensure compatibility with old G-Code programmes.<\/p>\n\n\n\n<p class=\"wp-block-paragraph\">The <strong>G84<\/strong>-command has the following syntax: <br><strong>G98(G99) G84 X Y Z R P F M<\/strong><br><br>The parameters for <strong>G84 <\/strong>are as follows:<br><strong>X<\/strong> - Position X<br><strong>Y<\/strong> - Position Y<br><strong>Z<\/strong> - Depth Z (absolute)<br><strong>R<\/strong> - Incremental value of the retraction plane in relation to the starting point in the Z-axis<br><strong>P<\/strong> - Waiting time in milliseconds (1000ms = 1sec.) at the bottom of the hole<br><strong>F<\/strong> - Feed speed in mm\/min<br><strong>M <\/strong>\u2013 <strong>M03 <\/strong>Right-hand thread, otherwise <strong>M04 <\/strong>Left-hand thread<\/p>\n\n\n\n<figure class=\"wp-block-table is-style-stripes\"><table class=\"has-fixed-layout\"><thead><tr><th class=\"has-text-align-left\" data-align=\"left\">Example<\/th><\/tr><\/thead><tbody><tr><td class=\"has-text-align-left\" data-align=\"left\"><strong>G00 Z0<\/strong><br><strong>G98 G84 X10 Y10 Z-10 F300 P100 M03<\/strong><\/td><\/tr><\/tbody><\/table><figcaption class=\"wp-element-caption\">Tapping cycle <strong>G84<\/strong> as right-hand thread<\/figcaption><\/figure>\n\n\n\n<p class=\"wp-block-paragraph\">In the above example, a right-hand thread (parameter <strong>M03 <\/strong>for clockwise rotation) with a depth of 10 millimetres and a feed speed of 300 mm\/min. At the bottom of the hole, a waiting time of 100 milliseconds (parameter <strong>P<\/strong>) is executed.<\/p>\n\n\n\n<div style=\"height:20px\" aria-hidden=\"true\" class=\"wp-block-spacer\"><\/div>\n\n\n\n<hr class=\"wp-block-separator alignfull has-text-color has-cyan-bluish-gray-color has-alpha-channel-opacity has-cyan-bluish-gray-background-color has-background\"\/>\n<\/div>\n\n\n\n<div class=\"wp-block-group alignfull has-global-padding is-layout-constrained wp-block-group-is-layout-constrained\">\n<p class=\"wp-block-paragraph\">We hope that this article will help you to quickly find your way around the world of drilling cycles.<br><br>Yours sincerely, Your BOENIGK-electronics Team<\/p>\n\n\n\n<div class=\"wp-block-buttons is-layout-flex wp-block-buttons-is-layout-flex\">\n<div class=\"wp-block-button\"><a class=\"wp-block-button__link wp-element-button\" href=\"https:\/\/www.cnc-controller.eu\/\" target=\"_blank\" rel=\"noreferrer noopener\">To the online shop<\/a><\/div>\n<\/div>\n\n\n\n<div style=\"height:100px\" aria-hidden=\"true\" class=\"wp-block-spacer\"><\/div>\n<\/div>","protected":false},"excerpt":{"rendered":"<p>In this article, we will take a detailed look at the G-code drilling cycle. You can then easily integrate these commands into your projects. Have fun reading!<\/p>","protected":false},"author":1,"featured_media":5369,"comment_status":"closed","ping_status":"closed","sticky":false,"template":"","format":"standard","meta":{"footnotes":""},"categories":[32,1],"tags":[35,14,36],"class_list":["post-5120","post","type-post","status-publish","format-standard","has-post-thumbnail","hentry","category-g-code","category-allgemein","tag-bohrzyklen","tag-g-code","tag-gewindebohrzyklus"],"_links":{"self":[{"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/posts\/5120","targetHints":{"allow":["GET"]}}],"collection":[{"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/posts"}],"about":[{"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/types\/post"}],"author":[{"embeddable":true,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/users\/1"}],"replies":[{"embeddable":true,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/comments?post=5120"}],"version-history":[{"count":0,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/posts\/5120\/revisions"}],"wp:featuredmedia":[{"embeddable":true,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/media\/5369"}],"wp:attachment":[{"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/media?parent=5120"}],"wp:term":[{"taxonomy":"category","embeddable":true,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/categories?post=5120"},{"taxonomy":"post_tag","embeddable":true,"href":"https:\/\/cncgraf.com\/en\/wp-json\/wp\/v2\/tags?post=5120"}],"curies":[{"name":"wp","href":"https:\/\/api.w.org\/{rel}","templated":true}]}}