Overview of CNC Milling procedures and issues

CNC machining to make wooden scale models is not an automatic process. Only some of the steps are semi-automated. How each step is executed determines what is possible, how long it will take to machine and what quality of finish will result.Although the procedures described here were developed for a particular CNC router (made by Techno-Isel), they are of general applicability. Like all such machines, the router has a gantry that moves over the working surface or bed in the y direction.Attached to the gantry is the spindle assembly that moves in the x-direction along the gantry.The spindle and the spindle motor, to which the drill-like cutter is attached, move up and down in the z direction on the spindle assembly. Each of the x, y and z directions of motion is provided by a dedicated servo motor.The spindle motor rotates the spindle at rotations up to 18000 rpm, in our case.

The overall procedure for milling an object is to create a threedimensional computer model of the object in three-dimensional modeling software and then to export this model to software that allows the creation of tool paths.Tool paths are instructions that tell the tool how to move in order to carve out the desired object from piece of material referred to as the stock.The instructions thus produced are in a generic set of codes called G-codes stored in text file format. Before the milling machine can execute the G-codes they are converted to machine specific instructions by the machine interface software that resides on the on-board computer that drives the milling machine.The software makes use of a controller card which sends signals to the controllers that control the motion of the servo motors which, in turn, move the spindle assembly in the required x, y and z directions.

We highly recommend cutting a test model first. Pink, rigid insulation is an excellent material for cutting test models (though we do not recommend Styrofoam because of its granular structure). It is inexpensive and forgiving of mistakes in tool path strategy and machine operation.We have found that, in an academic setting, where each scale model to be machined is sufficiently different, cutting a test model wholly or partly is essential. So each of the following steps should be executed first with test material and then repeated with the real material. Occasionally, we also recommend cutting a partial model in the final material in order to confirm feeds and speeds and cutting strategies. Here is an overview, in more detail, of the steps we go through to mill an architectural scale model in wood.

1) Exporting to stl: Export the three-dimensional computer model to stl (stereo lithography format).This format is the most common format used for rapid prototyping of all sorts.The stl format represents surfaces as tiny triangles (For curved surfaces good stl representations use more triangles in areas of high curvature and allow the user to specify the chordal tolerance or error, namely, the distance from the surface of a triangle to the curved surface it approximates).The computer model must be the same size as the actual physical model to be produced.

2) Cut the stock: Cut a piece of material, called the stock, from which a scale model is to be machined.

3) Model the stock: Create a three-dimensional model of the stock that is exactly the same as the physical test stock.This model can be created in a three-dimensional modelling package or directly in the tool path software if the shape is simple.

4) Generate the tool paths: Use tool path generation software (we use Visual Mill but there are several others) to create the tool paths that will guide the CNC milling machine to cut the scale model from the stock.This process does not require knowing how to do program tool paths with Gcodes but it does require knowledge of the different tool path strategies and the appropriate tools to use for each strategy as well as associated parameters such as feeds and speeds to be used by the cutting tool. Feeds and speeds depend on the type of material being cut. For example, rigid insulation my be cut at high feed rates (the rate at which the cutting tool moves through the material to be cut) and high rotational speeds of the tool, whereas different kinds of wood each have a speed limit depending both on how fast the cutter can remove material as well as the heat produced (which can produce burning) and the type of finish produced. With basswood, for example, we often noticed fuzzy edges being formed which can be minimized by selecting appropriate cutting speeds.The values to use for feeds, speeds and associated parameters when cutting wood do not seem to be available in the literature or on the Web.The general feeling among CNC users cutting wood seems to be that the values are so case specific that they must be determined by experience.The closest we have come to finding any recommendations was for cutting large sheets of thick plywood with fairly large diameter cutters.We found these speeds to be much too high for cutting curvilinear models in basswood, for example.

Tool path strategy refers to the fact that there are different ways that the cutter can be programmed to remove material to produce the desired shape. For example, in parallel machining, the cutter moves in parallel paths following the x or y coordinate directions with each path overlapping the previous by a specified amount. For parallel machining of curvilinear surfaces, the tool used is likely to be a ball nose cutter (a drill bit-like tool with a round end). Usually, a tool path strategy involves several different machining operations ranging from rough cut operations, with a large diameter, flat-bottom tool, to finish operations with a smaller diameter ball nose cutter.

When deciding on what tools to use for different tool path strategies and on the strategies themselves, consideration must be given to clearances. For example, will a given length of cutter allow cutting a valley of a certain depth without the tool spindle assembly or the collet (the part of the spindle which actually secures the tool) striking material that has not been cut or striking the clamps that secure the stock to the work surface? The final surface finish of a curved surface is determined by the size of the scallops (valleys with a semi-circular cross section and sharp ridges between valleys where the valleys intersect each other) resulting from parallel finishing.The height of the ridges can be calculated from the spacing between parallel cuts and the radius of the end of the cutting tool according to the formula: D = 2 (2rh – h2) 1/2 where d is the stepover distance between cuts, r is the radius of the ballnose of the cutter and h is the scallop height.A light manual sanding operation will remove the scallops altogether if the scallops are sufficiently small.

5) Securing the stock: Securing the stock to the work surface does not at first seem to be a significant issue or to require much planning. In fact, how a stock is secured is very significant because it is possible for the cutting tool to run into the clamps when trimming the sides of the stock. For this reason it is good practice to place some wood blocks between the metal clamps and the stock in case the cutter does accidentally move into this location. Ideally, careful planning of tool paths and setting of limit planes avoids such problems.When cutting large surfaces from flexible materials it is not sufficient to only clamp the edges. For such situations, a vacuum working surface allowing the flexible middle of the stock to be sucked down against the surface is useful.

6) Setting the origin. Generally it is customary to set the coordinate system origin at the lower left of the top surface of a rectangular piece of stock.This position avoids accidentally cutting into the stock during a horizontal motion to the initial milling position (if other precautions have not been taken). Ideally, one should create the three-dimensional computer model in such a way that it includes some stock that will not be cut away. That will allow the selection of an origin that will remain throughout the milling process. If the intention is to rotate the stock to the other side in order to mill the stock from two sides, we have found that it is easiest conceptually to locate the origin on the axis of symmetry on the top surface, that is, on the middle of the top left edge.To position the tool precisely at the origin we have been using a very straight nail (with head removed) secured in place of a cutting tool so that the x and y coordinates of the origin can be precisely located at the tip of the nail.We then replace the nail with the actual tool and locate the z value of the origin at the value where a piece of paper can just be moved between the surface of the stock and the tip of the tool.

7) Changing tools:After each milling operation, the tool must be changed. Each new tool is likely to be of a different length thus requiring a change in the z value of the origin to be set. Our technique is to move the tool-holding assembly away from the stock, insert the new tool and reposition at the x, y location of the origin over the stock We then lower the tool slowly to the surface of the stock, so that a piece of paper can just barely be moved between the tip of the tool and the surface of the stock. Finally, we reset the z of the origin to zero in the machine interface software.

© 2017 Privacy Statement Facebook Building your CNC router