Over the past three weeks, we made: the CAD molds for the body, top camera piece, and bottom camera piece; the CAM for the body, bottom camera piece, and top camera piece; and the molds for the body, bottom camera piece, and top camera piece. From the many hours spent manufacturing and the mistakes made we developed a better understanding and intuition for machining. We also faced several complications with the injection molding process including the misalignment of the cavity and core of our body mold; the acquisition of the right sized dowel pins; and the destruction of two tools CAM wasn’t set up correctly. Despite these obstacles, we tackled them, adjusted, and learned from them. We injection molded the body piece and began to understand how to tweak the settings to get the best possible part outcome. The Yolaroid is close to its first assembly run.
Machining Experience
Using the mill proved to be a time consuming task. With the entire team having little milling experience, machining was very slow at first. Initially, the entire set-up took around 45 minutes. However, once we got going, things went smoothly for the most part. Machining comes with a lot of feel and intuition, two things all of us lacked due to our little exposure. Overall, the entire experience came with a lot of mistakes, but also a lot of learning opportunities.
Exporting Our Files and Learning to Set the Z Height
Machining Experience
Using the mill proved to be a time consuming task. With the entire team having little milling experience, machining was very slow at first. Initially, the entire set-up took around 45 minutes. However, once we got going, things went smoothly for the most part. Machining comes with a lot of feel and intuition, two things all of us lacked due to our little exposure. Overall, the entire experience came with a lot of mistakes, but also a lot of learning opportunities.
Exporting Our Files and Learning to Set the Z Height
Once the CAM was finished for either the cavity or core of the part, we would use the post-process operation to export our G Code into the “.gcd” extension. Using a flash drive, we would transfer the file over to the mill and navigate through the menus to select the file and open it. Simultaneously, we would also install our core, cavity, or both on the fixture using ¼-20 screws and a 5/32” allen key. One thing we learned quickly was that the machine has programmed offset heights in it for a set of tools that allow the machine to understand the Z axis absolute zero that you set at the beginning of the operation. The machine also recognizes when you are using the quill to adjust the Z and takes this into account as well; as a result, you can use the quill to “touch off” the top of the piece and trust that the machine knows where the zero position is set.
One mistake that was made early on was thinking that the two mills had the same set of tools. We quickly realized this wasn’t the case when we tried to use the tools associated with the other machine and noticed that the heights were significantly off. Rather, each machine comes with its own set of Prototrak tools with offsets already programmed into the machine. We also learned that we needed to use the correct G codes to indicate whether the CAM should be completed on the core or cavity. In Fusion, this meant assigning each piece with a 2 or 3, to indicate core and cavity, respectively. In the G Code, this would show up as G55 or G56, respectively.
Edge-Finding
The edge-finding process was used to define the X-axis and Y-axis origin on the machine. Throughout this process, we used the machine’s jogging capabilities to get us in the vicinity of the area where we needed to touch off. We learned that the jogging setting is extremely helpful, but can be detrimental if we forget that we are in that setting and try to touch off, causing the tool to crash. Upon finally using the tool, the spindle speed was set to approximately 1200 rpm, and when finally detecting the edge, the X and Y parameters were set with an offset of 0.1’’ to account for the diameter of the edge finder.
One of the problems that arose from edge-finding was using the cavity or core block as the origin of our X and Y axes, when in actuality, the origin is the top right corner of the structure holding the cavity and core blocks in place. The corner is marked with an “x” to emphasize that the origin should be set in that spot.
Starting the Machine
Once everything was loaded onto the machine and the origin was correctly set, we needed to actually run the job. After proofreading and verifying the G Code, the correct tool for the first task was inserted, taking care not to get any body parts caught on the machine. Then we would hit “run” on the machine and “start.” After, we would turn on the spindle and proceed as we held onto the joystick, where we could pause to verify the actions and restart the program as necessary. For each tool path, the feed rate was reduced to approximately 30%-40% to reduce the amount of force acting on the tool. A lower feed rate resulted in a longer machining time, but it reduced the risk of breaking a tool. Typically, after bringing the feed rate down, it was brought back up to around 50% to 70% but never to its full potential. The spindle speed was not tampered with.
We learned to pause frequently — many times, we were able to catch other mistakes (such as edge-finding in the wrong location) by observing that the machine seemed to be about to drill in the wrong location, or noticing right away that a drill was not pecking. For example, pecking is essential so that the entire drill bit is not used being used to cut at once and instead cuts incrementally. This prevents wear on tool. Therefore, especially at the beginning, our runs were very slow, and we constantly revisited our CAM as we realized the slight modifications that needed to be made. During one run, the tool offsets had not been loaded onto the machine, so we spent a long time re-entering those manually. Though it later turned out that we could have simply loaded this from the lab flash drive, the time we spent doing this cemented our understanding of how offset heights work. Now, while machining, the numbers on the DRO are actually insightful to us and can alert us when there may be an issue.
Milling Sounds
Listening to our runs helped us to identify problems. During one run, we heard a shaky vibrational noise. This alerted us to the chatter that was occurring from a given tool path! When we paused, we quickly realized that the characteristic grooves were present on the workpiece finish. We identified the cause: one of the screws holding the stock to the fixture had loosened, causing the mold to vibrate, so we simply tightened it to fix the problem.
We also occasionally heard a squealing tinge to the normal machining noise. We found that this indicated usually one of two things:
The feed rate was too low. Sometimes in our eagerness to be careful, we overrode the specified feed rate too much. Though the tool initially approaches the workpiece quickly, it innately slows down when it begins the cut. Therefore we eased up on the override and the machine noises went back to normal.
We also hypothesized that cutting the aluminum dry might contribute to the squeaky noise. For longer cuts, we added oil, either with the spigot or by brushing oil onto the tool head periodically to prevent chip buildup. In some cases, this also restored machine noise to normal.
The Benefits and Drawbacks of Fusion Simulations
Overall, the simulations in Fusion were very helpful. They provided insight on the path the tool would follow, and indicated any problematic regions where it might crash or not perform as expected. More specifically, the simulations were used to determine how much material each tool path would take off, so that we could determine whether it was necessary to adjust the current tool path to reduce the amount of material being cut or to add a new finishing pass to clean up the areas the tool path failed to reach. Simulations also helped us to realize that certain tools may never successfully perform certain operations. For example, we have several tight corners in our molds, which are obviously limited by the tool diameter. In our initial CAM, we would try to begin the cutting with a large adaptive tool path using a 3/8” tool, only to realize from the simulation that too much material was being left behind and that we should run a second path with a smaller tool.
Although proving to be very beneficial for us, there were some drawbacks and limitations to the simulation. One drawback was that Fusion 360 failed to have the correct tool height for T2 (1/16’’ flat endmill, long), so the simulations would sometimes portray the tool crashing even though in reality, the tool would be fine. It was a little disconcerting to ignore the warnings, but it also taught us to not rely fully on the simulations. One of the limitations of the simulation is that it cannot inform the user when a tool is going to break because it is taking off too much material at a time. As a result, it is important to have an intuition and understanding of the forces the tool is undergoing during the cutting process. Therefore, we treated the Fusion simulation as the first step in ensuring tool path success, but also combed through it ourselves to ensure that the correct settings were set. Sometimes Fusion did not anticipate a tool crashing, but in reality after measuring the tool heights and distance from tip to tool cone compared to stock height, we decided we were cutting it too close and opted for a different cutting path or tool.
Breaking Tools
During this process, we broke T2 (1/16’’ flat endmill, long) twice — sorry! When creating our first cavity mold, we accidentally broke the tool during a run when we forgot to lower our feed rate. We mistakenly thought that this had caused the breakage, so the following day after replacing the tool and re-touching off the Z, we repeated our mistake and broke the tool again. A bit more research and talking to the lab instructors revealed that the true cause of the breakage was that too much material was being taken off at once. Essentially, the entire length of the tool was cutting into our part — and given that T2 is already a long tool, there was too much load on the tool head.
To fix this issue, we added a few critical elements to our CAM. We changed the maximum and minimum stepdown to prevent the tool for using too much of its length at once. We learned that best practice is to use 10% of the tool length, which of course increased our machining times, but also ensured that we haven’t broken any tools since. For contour paths, we learned to double-check that the multiple depths feature was toggled on. In general, breaking the tools prodded us to comb through every menu option for the CAM and we now understand the settings far more thoroughly. We picked up on some other good practice techniques — such as setting axial stock to leave equal to 0, and turning on flat area detection — that we hadn’t explored previously.
G Code Analysis
Below is an analysis of a sample of G-Code used to make the Yolaroid Body Molds.
(DRILL10) → Indicates the type of tool being used
N0130 M01 → Optional Stop. Machine will stop until all conditions are ready for use.
N0135 T19 M06 → Change to tool 19.
N0140 T16 → Select tool 16.
N0145 S4775 M03 → Turn spindle on (clockwise) at spindle speed 4775 rpm
N0150 G55 → Use specific WCS offset.
N0155 G00 X1.0433 Y-0.6029 → Rapid positioning to destination point at X-coordinate = 1.0433 in and Y-coordinate = -0.6029 in
N0160 Z0.6 → Position at Z-coordinate = 0.6 in
N0165 G00 Z0.2 → Rapid positioning to Z = 0.2 in, moves drill down
N0170 G83 X1.0433 Y-0.6029 Z-0.4013 R0.2 Q0.03 F7. → Peck drilling cycle with full retraction pecks to destination point at X = 1.0433 in, Y = -0.6929 in, Z = -0.4013 in, with retract position in Z of 0.2 in, delta increment along Z-axis of 0.03 in, and cutting feed rate of 7 in/min.
One mistake that was made early on was thinking that the two mills had the same set of tools. We quickly realized this wasn’t the case when we tried to use the tools associated with the other machine and noticed that the heights were significantly off. Rather, each machine comes with its own set of Prototrak tools with offsets already programmed into the machine. We also learned that we needed to use the correct G codes to indicate whether the CAM should be completed on the core or cavity. In Fusion, this meant assigning each piece with a 2 or 3, to indicate core and cavity, respectively. In the G Code, this would show up as G55 or G56, respectively.
Edge-Finding
The edge-finding process was used to define the X-axis and Y-axis origin on the machine. Throughout this process, we used the machine’s jogging capabilities to get us in the vicinity of the area where we needed to touch off. We learned that the jogging setting is extremely helpful, but can be detrimental if we forget that we are in that setting and try to touch off, causing the tool to crash. Upon finally using the tool, the spindle speed was set to approximately 1200 rpm, and when finally detecting the edge, the X and Y parameters were set with an offset of 0.1’’ to account for the diameter of the edge finder.
One of the problems that arose from edge-finding was using the cavity or core block as the origin of our X and Y axes, when in actuality, the origin is the top right corner of the structure holding the cavity and core blocks in place. The corner is marked with an “x” to emphasize that the origin should be set in that spot.
Starting the Machine
Once everything was loaded onto the machine and the origin was correctly set, we needed to actually run the job. After proofreading and verifying the G Code, the correct tool for the first task was inserted, taking care not to get any body parts caught on the machine. Then we would hit “run” on the machine and “start.” After, we would turn on the spindle and proceed as we held onto the joystick, where we could pause to verify the actions and restart the program as necessary. For each tool path, the feed rate was reduced to approximately 30%-40% to reduce the amount of force acting on the tool. A lower feed rate resulted in a longer machining time, but it reduced the risk of breaking a tool. Typically, after bringing the feed rate down, it was brought back up to around 50% to 70% but never to its full potential. The spindle speed was not tampered with.
We learned to pause frequently — many times, we were able to catch other mistakes (such as edge-finding in the wrong location) by observing that the machine seemed to be about to drill in the wrong location, or noticing right away that a drill was not pecking. For example, pecking is essential so that the entire drill bit is not used being used to cut at once and instead cuts incrementally. This prevents wear on tool. Therefore, especially at the beginning, our runs were very slow, and we constantly revisited our CAM as we realized the slight modifications that needed to be made. During one run, the tool offsets had not been loaded onto the machine, so we spent a long time re-entering those manually. Though it later turned out that we could have simply loaded this from the lab flash drive, the time we spent doing this cemented our understanding of how offset heights work. Now, while machining, the numbers on the DRO are actually insightful to us and can alert us when there may be an issue.
Milling Sounds
Listening to our runs helped us to identify problems. During one run, we heard a shaky vibrational noise. This alerted us to the chatter that was occurring from a given tool path! When we paused, we quickly realized that the characteristic grooves were present on the workpiece finish. We identified the cause: one of the screws holding the stock to the fixture had loosened, causing the mold to vibrate, so we simply tightened it to fix the problem.
We also occasionally heard a squealing tinge to the normal machining noise. We found that this indicated usually one of two things:
The feed rate was too low. Sometimes in our eagerness to be careful, we overrode the specified feed rate too much. Though the tool initially approaches the workpiece quickly, it innately slows down when it begins the cut. Therefore we eased up on the override and the machine noises went back to normal.
We also hypothesized that cutting the aluminum dry might contribute to the squeaky noise. For longer cuts, we added oil, either with the spigot or by brushing oil onto the tool head periodically to prevent chip buildup. In some cases, this also restored machine noise to normal.
The Benefits and Drawbacks of Fusion Simulations
Overall, the simulations in Fusion were very helpful. They provided insight on the path the tool would follow, and indicated any problematic regions where it might crash or not perform as expected. More specifically, the simulations were used to determine how much material each tool path would take off, so that we could determine whether it was necessary to adjust the current tool path to reduce the amount of material being cut or to add a new finishing pass to clean up the areas the tool path failed to reach. Simulations also helped us to realize that certain tools may never successfully perform certain operations. For example, we have several tight corners in our molds, which are obviously limited by the tool diameter. In our initial CAM, we would try to begin the cutting with a large adaptive tool path using a 3/8” tool, only to realize from the simulation that too much material was being left behind and that we should run a second path with a smaller tool.
Although proving to be very beneficial for us, there were some drawbacks and limitations to the simulation. One drawback was that Fusion 360 failed to have the correct tool height for T2 (1/16’’ flat endmill, long), so the simulations would sometimes portray the tool crashing even though in reality, the tool would be fine. It was a little disconcerting to ignore the warnings, but it also taught us to not rely fully on the simulations. One of the limitations of the simulation is that it cannot inform the user when a tool is going to break because it is taking off too much material at a time. As a result, it is important to have an intuition and understanding of the forces the tool is undergoing during the cutting process. Therefore, we treated the Fusion simulation as the first step in ensuring tool path success, but also combed through it ourselves to ensure that the correct settings were set. Sometimes Fusion did not anticipate a tool crashing, but in reality after measuring the tool heights and distance from tip to tool cone compared to stock height, we decided we were cutting it too close and opted for a different cutting path or tool.
Breaking Tools
During this process, we broke T2 (1/16’’ flat endmill, long) twice — sorry! When creating our first cavity mold, we accidentally broke the tool during a run when we forgot to lower our feed rate. We mistakenly thought that this had caused the breakage, so the following day after replacing the tool and re-touching off the Z, we repeated our mistake and broke the tool again. A bit more research and talking to the lab instructors revealed that the true cause of the breakage was that too much material was being taken off at once. Essentially, the entire length of the tool was cutting into our part — and given that T2 is already a long tool, there was too much load on the tool head.
To fix this issue, we added a few critical elements to our CAM. We changed the maximum and minimum stepdown to prevent the tool for using too much of its length at once. We learned that best practice is to use 10% of the tool length, which of course increased our machining times, but also ensured that we haven’t broken any tools since. For contour paths, we learned to double-check that the multiple depths feature was toggled on. In general, breaking the tools prodded us to comb through every menu option for the CAM and we now understand the settings far more thoroughly. We picked up on some other good practice techniques — such as setting axial stock to leave equal to 0, and turning on flat area detection — that we hadn’t explored previously.
G Code Analysis
Below is an analysis of a sample of G-Code used to make the Yolaroid Body Molds.
(DRILL10) → Indicates the type of tool being used
N0130 M01 → Optional Stop. Machine will stop until all conditions are ready for use.
N0135 T19 M06 → Change to tool 19.
N0140 T16 → Select tool 16.
N0145 S4775 M03 → Turn spindle on (clockwise) at spindle speed 4775 rpm
N0150 G55 → Use specific WCS offset.
N0155 G00 X1.0433 Y-0.6029 → Rapid positioning to destination point at X-coordinate = 1.0433 in and Y-coordinate = -0.6029 in
N0160 Z0.6 → Position at Z-coordinate = 0.6 in
N0165 G00 Z0.2 → Rapid positioning to Z = 0.2 in, moves drill down
N0170 G83 X1.0433 Y-0.6029 Z-0.4013 R0.2 Q0.03 F7. → Peck drilling cycle with full retraction pecks to destination point at X = 1.0433 in, Y = -0.6929 in, Z = -0.4013 in, with retract position in Z of 0.2 in, delta increment along Z-axis of 0.03 in, and cutting feed rate of 7 in/min.
Speeds, Feeds, and Other Parameter Choices
Overall, we agreed with the default spindle speeds on the CAM, except for the edge-finding tool. We set the spindle speed for the edge-finder to approximately 1200 rpm. This proved to be a happy medium to not wear down the sides of the tool but still manage to detect the the slightest deviation of the tip of the part. The default spindle speeds for the drills were 2000 rpm. This proved to be a perfect spindle speed enough for the drill to penetrate the material with adequate force but not so fast that the chips get adhere to the drill and damage it. The spindle speeds for the tools that were cutting the aluminum were set to 5000 rpm--the maximum spindle speed on the CNC mill. A quick calculation revealed that this was well within the acceptable range for our tools (Equation 1) given the suggested cutting speeds for HSS tools in an aluminum workpiece. Additionally, aluminum is a soft material and the tools being used are high speed steel; this allows for a higher spindle speed to be used without the tool burning up and wearing away. Furthermore, a spindle speed of 5000 rpm allowed the feed rate to be larger and the tool to cut with less of its diameter. A higher spindle speed may cause the chips to adhere to the tool but this was compensated for by adding oil and air to the tool as it cut.
The feeds were always lowered to 30% when actual cutting or drill ensued to be safe. A higher feed rate causes the force on the tool to increase, as a result, if the feed rate is too high this can cause the tool to break. This is a very common way tools break and has happened in the lab many times. Once the tool started cutting, we increased the feed slowly by 10% increments but never exceeded 60%. We increased the feed rate because 30% proved to be really slow for the tool and sometimes resulted in a high pitched shrill during the operation. Additionally, we reduced the feed rate to an initial 30% for safety concerns.
3D adaptive passes, 2D contours, and 3D finishes were always done at multiple depths and/or passes. Multiple depths were used to reduce the area of the tool that was actually cutting. The greater the area of the tool that was cutting, the more force the tool felt which could lead to the tool breaking, especially for smaller or longer tools. In consequence, the maximum stepovers were generally 10% of the tool diameter. The stepover could potentially be increased but the 10% rule is generally used just to be certain that a tool would not break. This was discovered when we broke two 1/16 flat endmills as described in the previous sections.
Overall Takeaways
One of the biggest takeaways that we learned from this experience is that, when it’s possible, you should machine an entire mold piece all in one sitting. There are so many minuscule differences in the edge-finding and changes in set-up that the best way to have a piece be consistent is to do it all in one go. There were several times that we couldn’t do this, due to our schedules or another team using the machine, but the ideal way would be to process everything together, so you minimize outside factors that might threaten consistency.
Injection Molding Experience
We injection molded our body part first using the BOY machine. We followed the step-by-step set-up instructions on the course website to mount both the core and cavity and determine the required ejector pin sizes. We also reamed the holes for the ejector pins and we tapped the sprue by hand before inserting the molds. After using the inserts to get the desired size of the ejector pins and installing them, it was time to place the molds in the machine. The very first time we tried to injection mold the body, we found that the core and cavity did not line up properly. We ended up re-running two operations on the core and got the desired results that we needed to fit the two sections together.
Then it was time to injection mold.
As can be seen in the photo on the left (our first trial), we experienced short shot due to insufficient packing pressure that meant that our part was not completely filled. In our next attempt at injection molding, we increased the packing pressure (according to what we found in the BOY manual) to force more plastic into the space and get more desirable results. We also knew that, as we continued the molding process, we would see lots of differences between the next several that we did, not just because of parameter adjustments, but also because the molds would be heating up. In between runs, they will not have the opportunity to cool down, so that will also affect the final product of each injection molding round.
In our next round, in addition to increasing the pressure, we also increased the cooling time by 15 seconds. We have a slot support area in our body that holds the photo that is a very large thick area. Typically, we should avoid these kinds of features because they are more susceptible to shrinkage and require us to increase our cooling time. The team is considering redoing that section and creating a new mold where ribs would be there instead, to achieve the desired support effect, but make the overall thickness of the mold more uniform.
Completing our molds and doing the injection molding process also highlighted some other issues that we might have. For example, our pegs came out very small, and we may need to lengthen them in future molds. We also saw a dishing effect along the outside edge of the yoyo body where there was caving in instead of a smooth surface (as shown in the below picture). This effect decreased when we increased the shot size, but then we also experienced minor flash, so there is a delicate balance to strike. As we continued making molds, the behavior of them changed due to the fact that the molds themselves did not have enough time to cool down. The behavior would have also changed if we had been using the bolt in the bottom of the yoyo as well. Through this experience, we have begun to understand how to optimize our parameters for the best results possible.
Comments
Post a Comment