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 the Biesse Woodworking Router with CIX Format.. We would be happy to get some feedback from you before we put them into production.
Feel free to download and test this post processor and provide any feedback you might have.
Thanks @reism1, any feedback you can provide is always greatly appreciated. The post is setup with the C-axis as being continuous (cyclic) so you shouldn't see any rewinds.
Hi community! I have been using this post for a while and after a little fine tune, I have to say that I feel so grateful about it and I'd like to let you know about a bug I have noticed and a suggestion. The bug, lately I have been dealing with an anoying issue that is blowing my mind. The milling functions work accurately, even in custom faces and the boring functions work properly on the standard faces. The party starts when I need a program in which I have boring functions and custom faces. I mean, if I have only milling operations on several custom faces, there is no problem. If I have only drilling operations on several custom faces, there is no problem. If I have milling and drilling operations on standard faces, there is no problem. But if I have drilling or milling operations on standard faces and drillings on custom faces, the thing becomes mad. Here I leave an example: This is what I program: https://ibb.co/VtHXxyj This is what I get: https://ibb.co/0D1gCgF As you can see, the drills get out of their place. If I deactivate the milling operations in the same file: https://ibb.co/Lp9FHj3 The drills return to thier place: https://ibb.co/8dKK5W3 I have to say that this example is made with the pure version of the post, so nothing related to the changes I made on it. Please, any idea about the cause of this issue? And the suggestion... Could it be posible to post process "CUT_GEO" macros? It is dedicated to made cuts with cutting discs. In my case I have patched this need creating a twin post in which the macros that are created for all the milling operations are named in the cix file as "CUT_GEO" instead of "ROUTG". This is a quite precarious solution, because now I have two posts, one for milling and boring operations, and another for disc cuts and boring operations. Certainly, this is not a good solution because I can't post process programs in which I have mill and disc cut operations together. The ideal solution would be that the milling operations programmed with a slot mill type tool were post processed as "CUT_GEO" macros. Do you think it could be made? Thanks in advance!!
I've tried the ISO-Postprocessor with Fusion360 and Inventor now. Both outcomes come alright when reading with HSM-edit, but when importing to my Rover C6.40, the code only says:
The ISO code is output in CONTORNATURA05 in the Biesse ISO post processor. You are showing the data output under CONTORNATURA01. Is there a way to select Contour 5 on the control? If not, you can try to cut-and-paste the G-code from CONTORNATURA05 into CONTORNATURA01 and see if this works on your machine. If it does, an option can be added to the post to select the contour # to output the ISO code to.
When using the .iso post I get an error message like this:
"Error: The post configuration requires revision 45500 or later of the post processor which has revision 42270. Failed while processing global script."
It is the post engine that is older than required by the Biesse ISO post. You are running an older version of HSMWorks or Inventor CAM and this needs to be updated to run this post processor.
So I did my first test of a program on my company's Biesse Rover S FT 1536 and was able to drag and drop the program into the workspace but it didn't recognize any of the tools that I had set. Is this just a matter of coordinating the proper tools in the proper tool holders or is there something else that I can do to communicate what's in the machine to HSM and vice versa? When the program loaded it looked like the toolpath and geometry was there but it asked to set the tool and depth for each operation. Any clues?
The name of the tool is output by the post right as it appears in the field "Product ID" when a tool is registered in Inventor CAM or Fusion. I guess the same for HSM. Make sure the "Product ID" in HSM matches the tool name in the machine.
Anyway, if that is not the point, upload a CIX file generated by the post and I'll try to help you with your issues.
I did what you suggested and input the product ID to match what the Biesse machine has each tool saved as and now when we pull up the program it recognizes the tools used. However, it's still asking for the depth to be set for each operation and it cuts along the centerline of the path instead of to the outside or inside that I set in HSM. I've attached the .cix file below. Thanks for helping me get the tool resolved at least!
When the cix file is generated, you get a polyline for each milling operation. Each one of those polylines is set in itself to a Z value according to the machining depth, so the depth must be set to 0 in bSolid or Biesseworks so as to not add longer depth. You can check at your machine software that you get something like this:
The blue line represents the toolpath already set at the right depth.
About the center compensation. You are getting a toolpath in which the offset compensation is already calculated in itself, so the same way that for the depth you have to leave it at 0 in the control, you also have to leave the compensation at centerline in the control.
If you want the compensation to be controlled by bSolid or Biesseworks, you must set the "Compensation Type" parameter in HSM to "In control".
I hope that helps you.
PS, when I've opened your CIX in bSolid I haven't had any issue with it, except obviously that I don't have any tool registered with your ID name.
@Rafa_Navarro wow thanks for clarifying this! I admit we never tried to run the program and I'm glad we didn't because we would have added even more depth to the cuts. I'll try this out and see how it goes. I guess the only drawback is that the operator doesn't see all the information beforehand but we can work around it. Thanks for your help and hoping this works!
Hi, 1st I am fairly new to Autodesk Fusion and Biesse works so I have big gaps in my knowledge.
I am generating the CIX file in Fusion 360. I take the CIX file to my CNC, open it Biesse Works, optimize and generate the ISO file, run the ISO file, works except for the order of operations. In the Fusion File, I have the tools in this order
5mm Drill
20mm Drill
3" Vbit
1/2 roughing
1/4 cutout
When I run my ISO (Also when I simulate in Biesse Works) "IT" does the holes, then starts with the 1/4" cutouts, then the 1/2" rough, and finally the Vbit. I dont know but seems to do the cutting in order of bit size. Just for the heck of it, I did try changing tool numbers around in fusion tool library, no effect. Still ran in the "wrong" order. I have also tried re - arranging the tool list in CAM, also tried deleting tool path and re creating them in a different order, same results.
I totally admit that I do not know if it is a Post issue or Biesse works issue.
I also generate a CIX file from my cabinet software, load it in Biesse works, generate the ISO and that works fine, cuts in a "logical order" - cut out the parts last.
Anyone have some suggestions for me?
BTW - I purchased the machine used so never have had much training on Biesse works
Hi, Just as an update in case anyone else finds this, see my post above.
Biesse works has a setting for the optimizer, and in my case it was set for time and was grouping all the 1/4" diameter cuts together to save time. Changed that and everything seems to be working great. Feel free to reach out if anyone has a question on what I did
Despite all the initial issues, I've been using this post processor with great success! I am running into a bit of a problem with the drilling operations though. Our machine has a separate carousel for the drill bits (actually brads) and for some reason it doesn't work when I program drilling operations in HSM using those tools. I'm kind of curious how the machine knows whether to call up the drilling tools vs. milling tools seeing how they have the same tool numbers. For example T1 is both a 3/8" endmill and a 5mm Brad depending on which carousel. Not sure if this is something I need to control in HSM or at the machine. Anyone have any insight? Currently I'm having to mill out all the drill holes which isn't ideal..
Have you assigned different tool names to the tools in the different carousels? It sounds like they may have the same name (T1). Be sure to match the tool names to you use in HSM (as described above by @Rafa_Navarro) as assigned on the machine and to enable tool name output with drilling operations.
@tgondek1970Having the same problem you're describing where the machine reorders my tool sequence. Can you give more detail as to how you change this setting? Seems like it wants to be changed to "work list" instead of by tool but I can't figure out where those settings are. Thanks!
Hi, Yes. Under I think its file, settings. Then go to the optimizer tab. From there there is a drop down menu for optimization type, and select "By Job List and head boring". That solved it for me 😉
I also had to change one setting in the post processor, it escapes me, I think it was something about tool names and BG macro. I believe it was a check box or a turn on / off option when I hit post in fusion.
Would be interested in knowing if that worked for you
Our woodshop is testing out software to program parts for our new Biesse Rover A, and I was really hoping HSMWorks would get us there, but I can't even get this latest CIX post to load into HSMWorks/Solidworks properly. I get this error each time! What am I doing wrong?
