LAZYCAM PRO + Polish overlay

Attention! Before purchasing a license, please read the product. and then make a wise purchase. because it is not possible to return the license.

When you purchase the program from our company, you receive technical support included in the price. We are the official distributor of ArtSoft software. On a daily basis, we assemble control sets for CNC machines. Over the years of working with the LazyCam program, we have become familiar with it :).

LazyCam (LC) from ArtSoft Newfangled Solutions is a simple, free program with which we can easily and quickly generate G-code, which we can then execute in Mach3. G-code generation is based on DXF or HPGL vector files. It is also possible to import graphic files, e.g. JPG or BMP. LC in the basic version is delivered together with the Mach3 program. It is possible to purchase the PRO version, which will enable the use of additional functions, such as: selecting pockets, creating offsets (tool diameter correction), preparing G-code for a lathe or a Styroplotter. If we use Mach3 in the demo version (without a purchased license), the generated G-code is limited to 50 lines.

We can install the LC software during the installation of the Mach3 program. We can also install it at any time. The LC installation file is located in the main Mach3 program folder (Standard: C:/Mach3). You can also download it from our website. When purchasing a license for the LC program, an overlay with the Polish version of the LC program will also be available.

LazyCam is a trial version of the software and no further updates are planned for it. Therefore, some functions may not work completely correctly. Before purchasing a license, please read the instructions for the LC software and test its capabilities to meet your needs.

To start working with LazyCam, we need a CAD program, e.g. AutoCad, in which we will prepare the tool path, saving it with the appropriate extension. Then it should be loaded into the LC program. When loading a project, we can choose from four operating modes: Mill (milling machine), Turn (lathe), Plazm (plasma). and Foam (styroplotter). Selecting one of the above operating modes will load the appropriate post-processor, which will allow the generation of G-code for the selected machine type. After loading the tool path, the program will automatically convert it into layers (Layers) containing all the details we want to process; hereinafter referred to as chains, which in turn consist of links (Entities). We will be able to set machining parameters for all these elements, such as: execution sequence, work speed, tool type, etc. We can also use one of the functions of the LC program, i.e. tool diameter correction (offset), pocket selection, or drilling. But more on that later.

It should be noted that the LC program is only used to convert a tool path prepared in a CAD program into G-code. We cannot edit elements there, apart from deleting them, changing their size and location. We can save the project at any time or send it to the Mach3 program, where we can simulate it or start processing a given element. Work simulation is also possible in the LC program itself.

The LC program can be launched from the Mach3 program. We can also use the shortcut we created. e.g. on the desktop. But. when we run the program with Mach3. then it is possible to automatically send the G-code directly to the Mah3 program. where we can test it. or perform. To run LC, select LazyCam in the File menu of Mach3. The absence of this menu means. that the LC program has not been installed. The installation file is located in the main Mach3 folder (LazyCamInstall file).

The window that will appear after starting the LC program is shown below. with Polish language overlay installed.

The view of the working areas of the LC program is presented in Figure 9 (page 13). At the very top we have the menu. with which we can set the program's operating parameters. Below we have a shortcut menu with the most needed functions. such as save/load project. undo changes. or generate G-code. In the middle of the screen there is a blue field where our project will be displayed. On the right side there is a toolbar with all the functions the program offers. The same functions are available in the Tools menu (function description later). On the left is the project window. where the layer tree will be displayed. Below this window there are buttons. that allow you to switch between additional functions. offered by the PRO version of the program. These include Pockets. Offsets (tool diameter correction). or Text (allows you to enter your own text). Below is the event bar. where messages related to all operations performed by the program are displayed. At the very bottom there is a status bar. which displays tips for most of the program's functions (the message is displayed when you point the cursor at a given function).
Using the View menu. and the Project and Info buttons can be turned on at any time. or turn off the display of a given window.

For the project window. and the event bar, we can use the mouse to change their position on the screen. By grabbing a given window by the blue bar, we can drag and drop it to another place. When you close the program, it will remember these changes and when you restart the program, the windows will be displayed in this way. what we set them before closing the program.

To fully use the functions offered by the program, we should use a mouse with a scroll wheel. The button assignments and keyboard shortcuts are described below:

We can select objects on the screen using the left mouse button. Clicking on the blue background will deselect them. Fast. double-clicking on a blue background will zoom out. or rotate the displayed toolpath.

Use the right mouse button to call up the pop-up menu. with which we can remove selected elements. or create. load. and remove the so-called templates – more on them later.

By pressing and holding the circle. and then moving the mouse will rotate the displayed toolpath. which will allow you to view it from different angles. We can then see, for example, the difference in the depth of layer processing.

We can turn it on using the S key on the keyboard. and turn off machining simulation (simulation time cannot be adjusted).

While holding down the Shift key. and then by moving the mouse while holding the left button we can zoom in or out.

While holding down the Ctrl key. and then by moving the mouse while holding down the left button, we can move the image in any direction.

Using the File menu, we can import a specific file type. whether to load the G-code file currently loaded into the Mach3 program. We can also save the LC (LazyCam) project. and then close the current project. or LC program.

New project – brings up a window. which allows you to create a new project with specific dimensions -
Open vector file – opens the window for loading a vector file, e.g. DXF. or HPGL-
Open image - opens the drawing loading window -
Open current… - will load the project currently loaded into Mach3 Mill. Attention. If G-code was loaded into Mach3 from LC. and then in Mach3 we manually changed the code. this is when we load the code from Mach3 to LC. he will take into account the changes introduced and modify the project.
Open LazyCam project – allows you to load previously saved LC-program projects
Save LazyCam Project As… - Allows you to save the current project with a specific name-
Save LazyCam project – when saved for the first time, it works like Save As. On subsequent saves, the program quickly saves
Close project – closes the current project-
Close program – closes the entire program.

Using the Settings menu, we can change settings related to automatic functions performed when loading the project into the LC program. and G-code generation.

Among the settings related to loading the project into LC. we can specify, among other things, what post-processor we want to use. It will allow us to generate appropriate G-code - tailored to our control (if we do not use Mach3, we can freely edit the post-processor - this topic, however, goes beyond this study).
We can also specify the place to save the created G-codes. add a name with automatic saving. add a comment in the form of the file creation date. As for the G-code itself, we can define it. how many lines should be numbered. whether to enable coolant service.

Plunge Clearance - determines the distance above the material at which the program moves from the cruising speed to the speed of entering the material when lowering the Z axis. The movement while lowering the axis is divided into two stages: Fast descent. and then delving into the material at the set speed. If the parameter is set to 0, the function is disabled. and the axis movement takes place from the Passing Height to the Cutting Depth (Cut level) with a constant defined speed of entering the material (Plunge speed). Below is an example G-code snippet. where the Plunge Clearance parameter was set to 1mm. Passage height at 2mm. a Cutting depth at -1mm:

N20 G0 Z2.0000 <-lifting the tool to the cruising height
N25 M3
N30 X1.0000 Y3.5000
N35 Z1.0000 <- quick lowering of the axis ( Plunge Clearance)
N40 G1 Z-1.0000 F60.00 < -driving into the material

Raising to the cruising height is done using G0 (rapid movement) then lowering the axis to the height specified in Plunge Clearance is also done using G0. From this point, the movement takes place at the set speed of 60 (using the G1 function).

Below is the same code snippet. except that the Plunge Clearance parameter has been set to 0.

N20 G0 Z2.0000
N25 M3
N30 X1.0000 Y3.5000
N35 G1 Z-1.0000 F60.00

How we see. the Z axis is lowered immediately at the set speed. using G1 (line N35 from the previous example is missing in this case).

Typically, feeds during fast passes (G0) are much faster than feeds during machining (G1). Defining the Plunge Clearance parameter allows you to speed up the machining process. related to lowering the Z axis (part of the downward movement may take place at a higher speed).

After selecting the appropriate functions in the export window, click Ok to save the changes.

Autosetting options allow us, among other things, to automatically optimize the tool path. If this option is not selected. then the cutting order will be consistent with what was loaded, e.g. from a DXF file. However, if the function is activated. then the execution order will be changed by the program. so as to obtain as few flights between objects as possible. It must be noted. that cutting operations are minimized in order to achieve the fewest tool changes. The cutting order can also be changed manually by the program user. More on this later in the manual.

Line Connection Tolerance function - determines the minimum distance between the ends of two lines in one layer. so that the LC program adds a pass-through movement between cutting them (if the distance is smaller than the given value, then the lines will be cut continuously - without passes between them).

The Tools menu allows you to select the functions offered by the LC program. These functions are also located in the toolbar on the right side of the main program window. These tools are available in each module of the LC program (milling machine, lathe, plasma). however, not all functions work in every module. The purpose of the function is as follows:

AutoSettings – performs the functions selected in the Settings/…AutoSettings menu (including: tool path optimization, layer regeneration, adding preparatory movements, changing the starting point).
Zoom - allows you to enlarge a selected area of the project. Indication is done by circling it. using the left mouse button. Double-clicking quickly returns you to the initial view (zooms out).
Delete chain - deletes the selected chain (a window confirming the deletion is displayed).
Set origin - sets the origin of the project to the minimum x and y values.
Scaling – a window is displayed. which allows you to scale the entire project. We can also convert units from mm to inches and vice versa.

Move chain – a dialog box appears. which allows you to change the position (within a given layer) of the selected chain using the mouse. or by specifying values for the X and Y axes by how much the object is to be moved. This function applies to text entered using the LC program.

It is also possible to move the chain to another layer. To do this, we must select a given chain in the project tree (left side of the program screen). Then right-click and select the appropriate menu: Move chain from new layer . or Move string to layer . In the new window, enter the name of the layer. that we want to use.

Set layer depth - this function allows you to quickly set the processing depth of a given layer (after selecting the chain, select the set depth function. Then, using the mouse, you can set the depth value - above or on the surface of the detail - by clicking the left button, you confirm the change). Another way to change the processing depth of a given layer is to go to the Layers tab. where we can define it. More about this in chapter 3.3.

Drilling holes – this function allows you to turn the selected chain (circle) into a drilling point. Not all CAD programs allow you to insert a point. and we can only draw a circle with a given diameter. To use the function, select the circle. and then click on the drill holes function. The selected chain will then be deleted. a point will be created in its place. which has been moved to a new layer called DRILL.

Remove the hole - the function works incorrectly - do not use it!

Rotate – calling this function allows you to rotate the selected object. or the entire project (when we select the rotate entire drawing function). Rotation can be performed using the mouse (by moving the mouse, we set the rotation angle and confirm with the left mouse button). or by specifying the rotation angle value.

Optimize the project – the LC program will automatically optimize the order of project execution. so as to achieve the minimum number of trips between facilities.
This feature is included in the Auto Setup feature. The order of project execution can also be determined by the program user himself.

Disable all introductions – will delete all introductions set by the program (Leadings).

Regenerate layers – the program will assign all objects to new layers. New layers will be created: Inside. and external layers (Outside). The inner layers will contain objects. that are contained inside other objects. These objects will be cut first.

Deselect all – calling the function will deselect all selected objects in the project.

Additionally, the toolbar offers the following functions (some of the functions overlap with those just discussed):

Drill holes in diameter - similar to Drill holes . With this difference. that brings up a window in which we can determine the diameter of the circles. to be converted into drilling points. All circles smaller in diameter. or equal will be converted into drilling points.

Delete points – this function allows you to delete drilling points created using the Drill holes function. and Drill holes with a diameter of .

Zoom – allows you to enlarge the area indicated with the mouse (hold down the left mouse button and then circle the desired area - double-click to return to the basic view).

Select – allows you to select several elements with the mouse (hold down the left mouse button and then circle the desired area).

Select inside – this function allows you to quickly select chains located inside the currently selected object.

Deselect – using the function allows you to deselect all selected elements in the project.

On/off flights – this function allows you to turn it on. or turn off the display of the tool path on the screen when moving between objects (visible as a dashed purple line).

Chain/Link - This function allows you to select a chain or link when selecting.

One/many - this function allows you to specify. Can we select one on the screen? or multiple objects (chain or link).

The View menu allows us to make choices. which windows should be visible in the program.

There are buttons at the top of the window. which allows you to perform the following actions:

Open .LCAM – a window will open. which will allow us to load the LazyCam project (we can save the progress of work with the LC program at any time and then load it to finish working on the project).

Open DXF – a window will open. which will allow us to load the vector file into the LC program. At the bottom of the window that appears, we can change the file extension. that we want to load: DXF. PLT. e.t.c..

Open the graphic - as above. with the difference that we can load images in JPG formats. or BMP.

Load Mach3 - allows you to load the project currently loaded into the Mach3 program. Same function as in the File/Open current… menu.

Save .LCAM – allows you to save the progress of the currently created project. so that you can come back to it at a later date.

Undo - this button allows you to undo the last change made -
Must be noted. that this option is possible for all changes.

Project – this button allows you to enable it. or disabling the display of the Project Window (same as the View menu).

Info – as above. except that it applies to the Event Window.

Generate G-code – the button allows you to generate a G-code.

Tabs are available in this window. that provide information about the program's operation. and about the currently implemented project.

The Project tab displays the history of activities performed since the project was created. There is a slider on the right side of the window. with which we can trace the history of work. if necessary.

After switching to the Extents tab, we can see the name of the loaded project. its minimum and maximum values in individual axes. the total number of chains. and links (Entities). The current coordinates of the mouse pointer position in the project are also shown at the bottom. At the top we can specify the connection tolerance (Cennection Tol.). which informs the LC program what the minimum distance between two cells is. below which the program treats them as connected.

In the Layers tab, we can define the processing parameters of a given layer. including: type of tool. working speed. cutting depth. or the so-called cruising altitude.

Before we discuss the Layers tab in detail, a few words of introduction about layers. As mentioned earlier. The LC program works on the so-called Layers. On the left side of the program window there is the Project Window. in which there is a tree with layers (visible after selecting the Project tab - figure below).

Each layer contains the so-called Chains (we can expand the layer on the tree using the plus sign). and chains contain. the so-called links (chain as well. we can expand it using the plus sign). Selecting the selected element (chain/link) on the tree. will highlight that item in the toolpath window and vice versa. selecting an item in the toolpath window. will highlight the selected chain/link in the tree. The program executes all elements of this tree from top to bottom. As already mentioned, the order of execution can be changed automatically by the program (Auto Settings function - the program itself will select the most optimal order of execution to obtain the fewest passes possible) - however, this function does not always work optimally. then we can manually change the execution order. If we grab a given element (layer/chain) with the left mouse button. then we can change their position on the tree. Whereas. when we right-click on the selected layer. or chain - then a pop-up menu will open with. from which we can remove the selected layer. optimize its execution. move the chain to a new one (here we must provide the name of the newly created layer). or to another. an existing layer (in this case we select a name from the group of existing layers).

In the Layer field of the Layers tab, we can specify the name of the selected layer. whether a given layer should be active. or not (read: done. or not). Disabling a given layer will result in that objects assigned to it will not be displayed in the toolpath window. and changes made to layers will not apply to it. Here we also have a preview of the order of execution of a given layer (numbering from 0).

The Layer Input Settings button launches the following dialog box. This button is also located in the Chains tab.

It's a window. allows us to determine parameters related to the so-called introductions – preparatory movements. and what type of processing will be used. Introductions are used when creating offsets.
LeadIn Size – determines the size of the introduction. It should be at least the diameter of the tool.
The LC program allows you to select several types of inputs: Straight. lines 45 deg. and Circular (arch).
Selecting the Leadin ON function – enables the leadin function for a given layer.
Outside/Right – determines the way the introduction is added.
Auto – the LC program automatically decides on the input settings.
Inside/Left - determines the way the introduction is added.
Climb Mill – we define the type of machining used for a given layer (for Climb the tool works opposite to the feed direction, while in conventional machining the spindle rotates in line with the feed direction).
OK – confirms the changes made.

The above settings are also available in the Settings/Charging Options… menu.


After selecting the above function. an introduction will be added automatically for the selected chain. which will be selected based on the entered size. or based on string size (default 10%).

For example. when we choose the Straight input type (straight line). we will get:

The operator can influence the type of inputs used. and their location. By grabbing the input with the left mouse button, we can move it along the outline of the selected chain and change its position.
By selecting the Off function We can delete the entries we have set at any time.
Worth noticing. that if there were no active introductions. in the same way, we can change the position of the tool entry/exit point on the material (in the tool path window, these points are connected by lines symbolizing through movement). Just grab it with the left mouse button and move it to the desired place. However, it is recommended. so that it is approximately the center of the selected chain (it certainly cannot be a corner of the chain). Please remember. that the change in the position of this point cannot be undone. After making changes that we are satisfied with, we should optimize the project.

In the Tool field of the Layers tab, we can preview the parameters of the tool assigned to a given layer. When we click on the Tool button. then a new window will open. with which we will be able to edit the tool parameters (Fig.15).

When we click the Create button then. a new window will open. where we can specify a name for the new tool. When we want to create a new tool. and we already have the tools defined. then we select one of the items on the list of tools on the left. before creating a new tool. This will copy the parameters of the selected tool to the newly created one - this may be useful. when, for example, we only want to change the name of the tool. Using the Delete tool button, we can remove the selected item. We can define the following parameters for the newly created tool:

Tool dia – tool diameter-
Post as Tool# - we can specify the tool number. which will be displayed in G-code-
FeedRate – we can define the feed at which a given layer is to be processed. The unit is units/min-
Plunge Speed - this is the speed at which the tool will penetrate the material -
Max Cut p/pass – we can determine what thickness of material is to be collected with one pass of the tool. This parameter is needed when working with multiple passes -
Spindle – we can determine the spindle speed. We should specify this parameter. if the program controls the spindle.

Before leaving this window, all changes must be confirmed using the Save parameters button - otherwise all changes will be lost.

Clicking the Set Layers button will assign the selected tool to all layers in the project (active ones). Do not click this button. if we want to assign the tool only to the currently selected layer.

In the Cutting field of the Layers tab we can specify how. the tool should move during operation.

Passing height – this is the height at which the tool is to move above the material. during passes between cuts.
Starting height – this is the height above the material from which we want to start processing the material (usually takes the value 0).
Cutting depth – determines how deep the detail is to be machined (it should be a negative value). This parameter is related to the Max Cut p/pass parameter (Fig.15) - based on these two parameters we determine how many passes a given passage will be made. For example. if we defined. that the cutting depth of a given layer is 10 mm. and the Cut p/pass parameter was set to 2mm. then the program will repeat the journey 5 times. each time collecting 2 mm. to obtain the set depth of 10mm.

Clicking the Set Layer button will assign the entered depths only to the currently selected layer. The Set Layers button will set all active layers. It is suggested. to set processing parameters for each layer separately.

Worth noticing. that when we import e.g. a DXF file into the LC program. then the program adopts the default tool (along with its parameters). and default depths for the Z axis for each layer/chain yes. to be able to show through movements. The program sets the speed of entering the material (Plunge speed) at 60 units/min. the value of material collected per pass (Cut p/pass) is infinite. and the cruising height has the value of 1 unit (mm or inches - depending on the Mach3 program configuration).

If we do not parameterize according to our needs. then G-code will be generated with these parameters.

In the Cutting field, we can also specify whether drilling is to be performed (G81 drilling cycle). or not (Nocycle). G83 cycles. and G73 do not work (will not be included in the generated G-code). If you need to change the drilling mode. then we have to do it manually in G-code.

The next tab of the Event Bar is Chains . where we can preview the parameters of the currently selected chain. which consists of a group of cells. The information displayed will change. when we select another object. whether on the project tree. or toolpath window.

The last tab from the Event Bar is the Entities tab. which allows you to view the parameters of the currently selected cell. The information displayed will change. when we select another object. whether on the project tree. or toolpath window. Links are individual elements that make up chains. These are objects of the type: arc. line (episodes). e.t.c..

Fig.18. View of the Entities tab

As already mentioned, tabs are available in the Project Window. which offer additional features of the PRO version of LazyCam. These will be tabs:

The first tab in the Project Window. which will be discussed in this chapter will be Pockets . When we select it, the window below will appear. The function is only active in the PRO version of the LC program (license required).

This function is used to create the so-called pocket. The procedure for using the function is as follows: select an object in the tool path window. for which we want to make a pocket. Then we define the function parameters (more on this in a moment). finally, click the Create Pocket button.


When we do this. then the program will automatically add the tool path like this. to fill the selected area (the tool will select the pocket according to the set depth by moving around it). In this function, we can define the following parameters: in the first step, you need to specify whether the selection should be done in a spiral manner. or zigzag (the type of generated trajectory depends on it). If we specify. that the selection is to be done in a spiral, then we must define the method of tool operation (CCW - tool operation counterclockwise - CW - clockwise) -

In-0ut/Out-In – here we define the direction of work – from inside to outside. or from outside to inside.
If we have chosen the second option, we must specify the angle at which the tool path is to be generated. 0 degrees defines the horizontal lines. 90 degrees defines vertical lines. We can also generate a path in the form of a grid. by using the Pocket function several times.


Just like for example. where a pocket was used for 0 and 90 degrees.

The next step is to select a tool (Tool button). The same dialog box will open. which was discussed when discussing the Layers tab (Fig.15).


Next, we have a preview of the parameters used to generate the pocket path.
Tool Dia - diameter of the tool used-
Step – we define how much subsequent passes of the tool should overlap the previous ones
OverHang – this parameter is inactive-
Finish – how much material is to be left (the excess that will be collected during the finishing move)-
Use Clamps – the LC program allows you to define the so-called clamps (these are objects that symbolize in the program how the detail is mounted on the machine - when we use them, the program will generate a tool path in such a way that it will allow us to change the position of the mounting and complete work in the places where the mounting was just located) . The exact use of the function will be discussed in the next chapter-
Create Islands – if there is another object inside the selected object for which we are generating a pocket. when we select this function. the path will be generated this way. to bypass an internal object. which will create the so-called island.
Based on the defined tool diameter. and other parameters, the LC program will generate a tool path after clicking the Create pocket button. The path will be displayed in the main program window. and in the project window on the tree. where new layers will be created (Pocket. and Offset). In the figure above we see the Pro Demo button…
instead of Create a pocket – this is the view we will see. when we do not have a purchased license. Then we cannot use this function.

It must be noted. that this function does not work completely correctly. When we choose the Spiral pocket option. is a CW/CCW selection. and Left/Right does not change the direction of the track. In-out/out-in function works properly. Due to an error, the path will continue to be generated. as if the CW direction was set.

And because the direction of work affects the type of machining. then we will still be dealing with conventional milling (the tool moves in the direction of feed).

Another error that may occur when using the pocket generation function is the lack of through-motion generation. The following screenshot of the LC program illustrates this.

The arrow indicates an error. The cruising altitude is set to 0 which will result. that during this movement the tool will pass over the material. To correct this, we must manually go to the selected layer. and then define the appropriate cruising altitude. Another way to solve this problem would be to use the Regenerate Layers function. Please remember though. that in this case the program will also automatically change all the names given to the layers.

Example of using the island-aware pocket selection function:

When you select an external element in the project. and activating the island function (Create Islands). when we click Create pockets, we should get the result as follows:

When discussing the Pockets function, it was mentioned. that the LC program allows you to use the so-called braces – these are objects. which symbolize in the program how the detail is mounted on the machine. During tool path generation. the program takes into account the presence of fasteners for the workpiece. The G-code is generated this way. to allow processing also under the fastenings. The processing is divided into two stages. First, the material not covered by fasteners is processed. When this piece of code is executed. work is stopped. The operator has time to change the position of the mountings. after which work can be resumed. where the processing of the detail is completed under the fixtures that have just been removed.

To create a mounting symbol. we must first create it in a CAD program. For example, let it be a square. Then we load our project into the LC program. Now we select our selected chain. right-click and select Save String as Template . In the window. which will now appear, we provide a name for the template. e.g. 25x25 clamp. Confirm your selection with the OK button. The color of the selected chain changed to yellow. From then on, it is a symbol of attachment. In this way, we can create a library of fasteners of various shapes and sizes. which we can use at any time. To do this, simply right-click and select Load saved template . A window with previously saved templates will open. We need to choose the clamp we are interested in. and confirm the selection by clicking OK. The selected item should appear in the program.

It must be noted. that when creating a template from a selected element, the operation cannot be undone. and the selected item will no longer be visible as a toolpath.

After loading our template into the project. we can place it in the chosen place. We can also rotate it to any angle.

When we right-click and select Delete templates . this will remove all fixtures from the project (of course they remain in the previously created library). We can also remove individual braces using the Delete function.

Below is an example of the effect of using the pocket selection feature with attachment in mind. On the left side, with the Use Clamps function selected. and on the right without this function enabled. How we see. when the clamp use function is enabled, the program divides the processing into two stages.

Example of using the offset function:

We select the element. for which we want to add an offset and click Create offset. We should get a new element in the project.

Above on the right we see the effect of using the function in question. The original element is marked in red. and a new toolpath surrounds it. taking into account the tool diameter. It is outside because we chose it. so that the offset is external. Similarly to the Pockets function. here also in the Project tab of the Project window. a new layer called Offset# will appear in the project tree.

If we set an offset for a given element to the original, we will most likely want to delete it. If we don't do it, it will also be executed. The situation is similar when creating pockets. We can remove the original shape. because the outer contours of the pocket will give us the original shape.

If we have a circle for which we want to apply the Offset function. and selecting pockets. then we first create the offset of the element. then we delete the original. And finally, we create a pocket.

It was mentioned above. that when using the offset function, we must determine, among other things, the direction of work - clockwise or counterclockwise. If we select the chain and zoom in on the spot. where the movement of raising/lowering the tool is performed, we will see an arrow showing the cutting direction. We can also know the direction by observing the order of links in the project tree. We can change the direction of work by specifying the type of work (Climb or conventional). using the Input Settings button.

The last tab from the Project Window. which will be discussed is the Text tab. It allows you to enter text to be cut from the LC program. This function is also available without a purchased LC program license.
After selecting the Text tab, you will see the window as below.

This function. allows us to choose the font type. which text will be entered. Then we need to enter the text in the text box. When you click the Place Text button. use the mouse to determine where to place the text. and its size (by selecting a rectangle of appropriate size with the left mouse button). Finally, we must define how we want to execute the entered text. Using the move/rotate function, we arrange the appropriate text characters. We can also use the pocket/offset function. We also cannot forget to define the tool parameters in the Layers tab. Depending on the selected font type, we will achieve a different end result.

Once we have determined all the necessary processing parameters. all we have left to do is generate G-code and execute it.
Now using the Post Code button (Generate G-code) we can generate the code. According to the settings, a message about generating a G-code will be displayed - named. as it was given to him. If the Mach3 program is running. our G-code should be automatically loaded into it. Now we can run a simulation of our project in Mach3. And if we are sure that everything is OK, we start the execution of the detail.

When working, remember that. at the top of the screen there is an undo button. with which we can undo the changes made at any time. We can also save our project at any time using the Save .LCAM button. so that you can come back to it at a later date and finish it. It is advisable to use the save before making changes. where we are not entirely sure of the impact on the project. This will allow us to easily restore the project in case of failure.

We encourage you to read the LazyCam user manual. At this link you will find a tutorial that describes in detail how to use the pocket selection function offered by LazyCam after purchasing a license.

If you have any problems or questions, please contact the technical support department at ebmia.pl. Any questions or comments can be sent to [email protected]. Also those regarding the edition

Claim orders from Stores

You can claim your purchased items within 1 - 4 work days after making an order (if product is in local warehouse).

Please wait for an email notification regarding Your order status update.

Vilnius Store address: Vytenio g. 20, LT-03229 Vilnius, Lietuva

Kaunas Store address: Pramonės pr. 4D, LT-51329, Kaunas, Lietuva

Local delivery in Lithuania

Purchased items are delivered locally through Venipak service. Depending on availability of items, orders are processed within 1-3 work days. Orders made until 1AM are shipped the same day.

Local delivery  (1-4 w.d.) price for items of any size is through through courier service is 4.90€ (incl. VAT), if the amount of the shopping cart exceeds 150€ - delivery is free.

Local delivery price to Venipak parcel terminals (1-3w.d.) is 2.90€ incl. VAT, if the amount of the shopping cart exceeds 50€ - delivery is free.

Local delivery price to Omniva parcel terminals (1-3w.d.) is 3.90€ incl. VAT,if the amount of the shopping cart exceeds 70€ - delivery is free.

Payment on delivery (COD) +2.00€ (incl. VAT).

You can pay for the goods at the time of delivery to the courier in cash or by credit card. Payment to Omniva parcel terminals is only possible by bank card.

A separate delivery fee applies to oversized items, regardless of the amounts and conditions stated above.

International delivery pricing through courier service

International shipping prices depend on geographic location:

Latvia - 5.50€ (incl. VAT)

Estonia - 6.50€ (incl. VAT)

Paid orders of more than 150€ are shipped for free to Latvia and Estonia.

other countries - negiotiated individually.

International delivery pricing to Omniva/Venipak parcel terminals

Latvia - 6.00€ (incl. VAT)

Estonia - 8.50€ (incl. VAT)

Payments:

We accept payments via PayPal for orders over 20€.

Product availability status:

Vilnius Store In Stock - the product is at the store, Vytenio str. 20 in Vilnius and can be picked up / purchased at same day;

Kaunas Store In Stock - the product is at the store, Pramonės pr. 4D in Kaunas and can be picked up / purchased the same day;

Central Warehouse In Stock - In stock, product will be shipped in a short time 1-2 work days;

1-2 work days - product will be shipped in a short time - 1-2 business days;

2-3 work days – we don’t have selected product in local warehouse. Shipping time is only 2-3 work days;

3-5 work days – we don’t have selected product in local warehouse. Shipping time is between 3-5 work days;

3-7 work days – we don’t have selected product in local warehouse. Shipping time is between 3-7 work days;

Out of Stock – selected product is sold out at the moment, but you can apply for automatic alert by email when product will be in stock.