Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
We are working on a generic post processor for an Okuma LB3000 Mill/Turn with an OSP-300 control. We would be happy to get some feedback from you before we put it into production.
Feel free to download and test these post processor and provide any feedback you might have.
I would like to request a few things that I believe would benefit the community.
1. At go home after a tool runs, there is nothing to send the Y axis home. This causes an error when a tool has a Y axis shift in the offset. The turret will not index until Y is homed out.
2. Load monitoring. Currently I have to use Pass thru in order to control load monitoring.
3. Sequence numbers increment by tool path when "Sequence numbers on tool change" is selected. I request that the numbers are only output at the tool changes.
4. Request separate sequence number start point for sub spindle
@Anonymous Thanks for the input. I do have some questions on some of your requests.
The post will be updated to send the Y home at a tool change.
Can you provide sample code for load monitoring and describe any values output that should be user definable (such as adding a new property).
This is considered a "user preference". Code was added specifically to output sequence numbers on operations that do not have a tool change. You can modify your post to not output the sequence numbers on operations without tool changes. I can provide assistance if you need it.
This is also a "user preference" and can be added to your version of the post.
Please don't hesitate to reach out if you require any further input or code samples.
Below is the load monitoring description.
I honestly haven't found good reason to use anything except spindle, x, and z axis monitoring at this time, but I have included the details from the manual describing how to use it.
I will try to figure out the sequence numbers, but may call on you for assistance if i need help.
2. Directly Below is the code that we'd use for OD turning tool T010101. Beneath that is an excerpt from the manual describing the monitor in detail.
(At begining of tool)
VLMON[1]=3 (load monitor on [tool number], limited to a range of 1-64 3=x & z monitoring. M216 (ignore load monitoring on rapid)
(at end of tool)
VLMON[1]=0 M215 (load monitoring on rapid on)
VLMON [part number] = monitored axis number Part number: 1 to 64 Monitored axis number: To monitor the load on two or more axes simultaneously, specify the sum of the relevant monitored axis numbers. Example 1: To simultaneously monitor the loads on the X and Z axes at turret A, the sub spindle and the W-axis, specify as follows: VLMON [ ] = 1 + 2 + 32 + 64 = 99 Example 2: To simultaneously monitor the loads on the X and Z axes at turret B, the M-tool spindle, and the Caxis, specify as follows: VLMON [ ] = 1 + 2 + 4 + 16 = 23 0 ... Load monitoring OFF for all axes 1 ... X-axis load monitoring ON
You can drill using the main spindle by unchecking the Live tool box in the tool definition of the drill.
When you say from the side, is the tool along the X-axis of the machine or the Z-axis?
If the tool is along the Z-axis, for radius programming are you using Polar Interpolation (G137), XZC mode (G101), or XYZ mode (G01)? The post will output the X-axis in radius mode for Polar interpolation and diameter for XZC and XYZ modes.
If the tool is along the X-axis, then it always uses diameter programming. Either way, you can modify the post to output the X-axis in radius mode for your case, just let me know which orientation the tool is in.
The problem was the x axis limit set to 0. The problem was the x axis limit set to 0. I have real value - 50. The next question is to delete the radius offset when milling. I have two milling operations with radius compensation. The first one he does correctly in the second one does not see compensation.
The problem occurs when it is one tool all the time. When I insert the operation with another tool, everything is ok.
Hi @bob.schultz , I am also running into a similar problem with x axis milling. Machine is an Okuma lb3000 ex ii. When i post out milling in the y axis it is doubling the x axis value. not sure if this is something that can be changed on the post, a setting i need to change on the machine, or something different i need to do with machine set up in fusion.
Hello @RYANKTOOL , thanks for reporting this issue. You are correct the post should be outputting the X-axis in radius mode and not diameter mode when the Y-axis is enabled. You can fix this in the post by adding these two lines in the getCode function.
case "ENABLE_Y_AXIS": setRadiusDiameterMode("radius"); return 138; case "DISABLE_Y_AXIS": setRadiusDiameterMode("diameter"); return 136;
We will get it fixed in the library version of the post.
Hey Bob, I use double stack tooling and I need the turret to go home in Y. I just use offset 00 to go home. Example: G00 T0100 Y0.
Also, could you make a safe start all operations function so that I can simply re-run the finish pass if I'm using the same tool for the roughing pass.
Hello @SWMWSHOP3, have you modified the post to output the move to home in the Y-axis? If not, can you explain when the move to home needs to happen, for example prior to a tool change.
The addition of a safe start for all operations will take a bit of modification to the post so cannot really be explained here. We will add it to the library post.
