Post processor issue with drill block Andi Selexx
Hi,
I am pulling my hair out trying to get my machine operating.
An Anderson Selexx 3719 2008 machine was purchased second hand and had no CAD/CAM software on the machine.
I decided Enroute7 would be a good choice to use.
I have been trying for weeks to get the software to run on my machine.
Yesterday an Enroute technician tried to solve the issues with the post and managed to solve several issues, but is having problems getting the drill block code to produce correct Gcode.
Surely there are other Andi Selexx machines in the world running Enroute software.
I am in Australia and the time difference with the tech guys is proving impossible to get a timely solution.
I dropped back to an earlier version Enroute6, but this was worse. Several Gcode commands it produced were incompatible with my machine.
Anyone out there who can suggest what I do?
Gary
Re: Post processor issue with drill block Andi Selexx
What post processors (machine drivers) have you tried. We have (had) recently sold both our Omitech Selexx Pal machines (had them since new in 2005). (We still have the one, waiting for it to be picked up.) Omitech was a subsidiary for Anderson for quite a while before Andi rolled them into their own line. Our machines both had Fanuc controls with the 9 spindle drill blocks and an 8 tool changer for the spindles. We ran our machines using Enroute 3, 4, 5 and 6. How is your machine configured? What control does your machine have?
Have you tried any of the Omnitech machine drivers? I know that the Anderson drivers and the Omnitech drivers were not the same with some different sets of codes. What exactly are the problems you're having?
Re: Post processor issue with drill block Andi Selexx
Quote:
Originally Posted by
Todd Zuercher
What post processors (machine drivers) have you tried. We have (had) recently sold both our Omitech Selexx Pal machines (had them since new in 2005). (We still have the one, waiting for it to be picked up.) Omitech was a subsidiary for Anderson for quite a while before Andi rolled them into their own line. Our machines both had Fanuc controls with the 9 spindle drill blocks and an 8 tool changer for the spindles. We ran our machines using Enroute 3, 4, 5 and 6. How is your machine configured? What control does your machine have?
Have you tried any of the Omnitech machine drivers? I know that the Anderson drivers and the Omnitech drivers were not the same with some different sets of codes. What exactly are the problems you're having?
Hi Todd,
Our machine has a Fanuc PLC.
I have not tried any Omnitech post processors. It's surprising the Enroute tech hasn't suggested that..
I could write a book on all the issues we have encountered since choosing Enroute. We were promised there was a post processor for our machine.
Initially we set the units to millimeters, but the Gcode was resetting it to inches.
The tech has managed to fix most issues, but there are still some problems.
I tried selecting the order I wanted the toolpaths done, in Enroute software, but the program was completely ignoring the order selected.
There were 60 slots to machine out of the part and I wanted it done efficiently with minimal distance travelled. Even in simulation, the software would dart all over the table skipping nearby slots, only to come back to them later. With order set to 1. Drill 2. Strategy, it machined out some slots, carved out part of the text, machined out more slots, carved out some more text, finished slots, finished text.
I have given up trying toolpath order at present.
Even now on a part with text in 12 different locations, it does part of the text in each location, returning to every location to finish the text.
I am starting to think we made a mistake selecting Enroute.
I wanted to use Fusion 360, but it does not support drill blocks.
regards,
Gary
Re: Post processor issue with drill block Andi Selexx
hy gary :) i can help with a custom application, that will scan your code and identify operations ( by searching for home positions, etc ), then allow you to reorder them
for drilling, just use your cam as it is, and is posible to detect the faulty drill operation and corect the syntax to suit your machine, as long as enough data is there
as long as you know what g-code should be there, i can help you reach it / kindly :)
Re: Post processor issue with drill block Andi Selexx
Yes, I'm guessing your machine is the same as ours. The Selexx Pal model was sold under the Omnitech brand in the USA until very recently. (A 2008 machine for sure would have been painted orange and grey and had the Omnitech name on it here.) There have been a few versions of the Omnitech Selexx Pal Enroute driver made. We had one custom written for us when we started using these machines. I think at least one of the ones that currently ships with Enroute is the same or very similar to the one we use. Also earlier versions of this machine used a Siemens control, you don't want to use the post for that or the Omtitech Syntec (which is another control on a different machine.).
As to tool path ordering, it can be a bit of a challenge with Enroute. When outputting first choose the methods you want to prioritize the output order of the tool paths. In the output dialog window, select the Priorities button, then move the items in the list into the order you want to use to order the tool paths. Choices are Strategy, Tool, Pass, Object, Layer (I generally have them in that order but sometimes rearrange them.) The Strategy Order button lets you choose the order that different tool path types will be ordered, (This is where you tell Enroute if you want to do the drilling before the milling, engraving...) You should always check these orders before you output, because Enroute will reshuffle them every time you output a new job (tacking new strategies to the end of the list regardless of what you saved the default order as. Enroute will only reorder to your saved defaults if if you click the "Reset parameters using Preferences" button (the one with the P and the arrow pointing at 2 o'clock). The Tool Order button is where you can set the order of tools uses priority. If you have "Tool" first in the Priority tab, then the order you listed the tools will determine the tool path order. Another important option in the Priority tab, is the "Pass", moving this to the top of the Priority Order list will order the tool paths by their depth milled.
Also the maintain grouping check box below the lists can be helpful, or it can screw you up, pay attention to whether or not you need or want to have that box checked.
Then the "Object Order" tab this is where you can override Enroute's default "traveling salesman" order algorithm. I've yet to fully master or understand some of the options in this tab. Some of them simply don't seem to do anything useful if anything at all. But some such as by column or row are straightforward enough to make sense.
One final trick that can be helpful if Enroute is being exceptionally stubborn with the output order. You can move your items to different layers and choose the "Layer" option in the Priority tab and move it to the top of the list. Then Enroute will output all the paths on the 1st layer before it moves to the next layer... But you must have all of the layers you want to be output visible on the screen when you output. Layers that are hidden will not have their tool paths generated.
If the job is simple enough you can use the tool order button and manually click out the tool path orders, but you easily can waste a ton of time on this only to loose all of your work, by accidentally clicking on one of the tool order buttons in the output dialogue box or changing any of the tool paths or part positions in the file. And to make matters worse the manual tool path info is never saved so the next time you open the job it will all have to be redone.
Re: Post processor issue with drill block Andi Selexx
One more thing, The "Simulate 2D" button in the "Output Tool Bar" can be very useful for fine tuning your output order before you actually make the g-code file for the machine. It has all of the same output priority settings as the output dialog. And you can test and simulate the effect of those settings there. Once you have the output working like you want in the simulation. Then you can open the Output button and click "To File" button and the order should be the same as you set it the simulation.
Just remember the orders are never saved when you save a file. The order priorities are the same as the last file you output, with any new path or tool types simply added to the bottom of the priority list.
Re: Post processor issue with drill block Andi Selexx
Hi Todd,
Thanks for all the information and help.
Enroute could definitely make their software more user friendly and follow options chosen (and save manual toolpaths).
I will explore the suggestions you made. It seems drawing in layers may be the best solution, but if the software worked correctly, I would not need to use layers.
Thanks again,
