Howdy.
I just switched over from VM4 to VM5.
Now I've encountered some problems:
It seems that VM5 is (on my PC) much slower than VM4 was.
My PC is a Pentium 4 2.66 MHz / 1GB RAM.
The moulds we create are build out of 500+ surfaces.
The roughing mill is a ball-end mill, 8mm dia, the
finishing mill sometimes a 0.5mm with 0.05 stepping.
Sometimes VM5 seems to hang after processing up to an hour
for roughing with a 2mm ball-end, but does it anyway.
Sometimes after one hour for processing VM quits working with:
"A serious error...blabla". In both cases VM "eats" up to 2GB of
memory (Mecsoft: I can send you screenshots and the VM-file).
VM4 "needs" only about 10 min. for the same procedure without quitting?
How comes?
Is there a switch for changing the scroll wheel? All of my other softwares scroll in the opposite direction.
BTW: The postprocessor does not use the correct file name, it
uses allways (!) the VMtempacl.acl !!!
Best regards,
Lars
Performance ???
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Performance ???
Hi Lars,
Our internal performance tests show that the performance between V4 and V5 are almost exactly identical. The problem you are facing could possibly be due to the fact you turned on "Insert Cutter" on. In 4.0 we did not have insert cutter processing. In 5.0 we have added this automatic to detect areas where an insert cutter is leaving and ignore these cut levels. To improve performance please turn the insert cutter off and try it. Also make sure you have the latest service pack (SP3) from our web-site. This SP removes this functionality as an automatic feature. Please run these tests and post the results. If you are still running into problems, send us the file.
-- MecSoft Support
Our internal performance tests show that the performance between V4 and V5 are almost exactly identical. The problem you are facing could possibly be due to the fact you turned on "Insert Cutter" on. In 4.0 we did not have insert cutter processing. In 5.0 we have added this automatic to detect areas where an insert cutter is leaving and ignore these cut levels. To improve performance please turn the insert cutter off and try it. Also make sure you have the latest service pack (SP3) from our web-site. This SP removes this functionality as an automatic feature. Please run these tests and post the results. If you are still running into problems, send us the file.
-- MecSoft Support
Performance ???
Hi Joe,
I've already installed SP3. What does it mean, "Insert Cutter" ?
I have found nothing that sounds similar to "Insert cutter" ?!
BTW: The file was send to Datacad (Germany), maybe they send it to
you. Otherwise I'll send it. The file's size is 10 Megs or so.
Best regards
Lars
I've already installed SP3. What does it mean, "Insert Cutter" ?
I have found nothing that sounds similar to "Insert cutter" ?!
BTW: The file was send to Datacad (Germany), maybe they send it to
you. Otherwise I'll send it. The file's size is 10 Megs or so.
Best regards
Lars
Performance ???
I thought V5.0 SP3 a lot slower than V4.0 as well so I've just done some tests on a small two cavity mould I'm working on, the results are.
V5.0 time to load 3dm file 1.20 mins, for horizontal rough 6.12 mins, for horizontal finish 8.30 mins. The total time in task manager for the whole job 16.16 mins.
V4.0 time to load 3dm file 1.17 mins, for horizontal rough 3.05 mins, for horizontal finish 1.07 mins. The total time in task manager for the whole job 5.35 mins.
This is with a simple model with only 20 faces.
I noticed if you close the V5 file then reopen and regen the horizontal finish it only took 2.0mins not 8.30.
I'll send the rhino file a two knowledge base files for you to check, tolerance for VM is set to 0.001.
I also tried to do some pencil tracing with V5 it took 4.20mins and V4.0 1.15min
Mark.
V5.0 time to load 3dm file 1.20 mins, for horizontal rough 6.12 mins, for horizontal finish 8.30 mins. The total time in task manager for the whole job 16.16 mins.
V4.0 time to load 3dm file 1.17 mins, for horizontal rough 3.05 mins, for horizontal finish 1.07 mins. The total time in task manager for the whole job 5.35 mins.
This is with a simple model with only 20 faces.
I noticed if you close the V5 file then reopen and regen the horizontal finish it only took 2.0mins not 8.30.
I'll send the rhino file a two knowledge base files for you to check, tolerance for VM is set to 0.001.
I also tried to do some pencil tracing with V5 it took 4.20mins and V4.0 1.15min
Mark.
Performance ???
I have noticed the pencil with a flat cutter seems to read every seam on the mold.Causing major bottleneckage!!Seems the algo could just relax a bit,nice that it sees every nook and crany,but it needs to better realize the difference between a corner and a surface seam.
My generation times have been about the same from 4.0 to 5.0.Maybe a tad slower for 5.0 but I have been attributing this to the fact that the toolpaths are getting "smarter" and in turn require slightly more processing time..But the fact that you notice it crunches faster after its been shut down could point to a memory leak somewhere!!
Greg
My generation times have been about the same from 4.0 to 5.0.Maybe a tad slower for 5.0 but I have been attributing this to the fact that the toolpaths are getting "smarter" and in turn require slightly more processing time..But the fact that you notice it crunches faster after its been shut down could point to a memory leak somewhere!!
Greg
Performance ???
Hi all,
I have the same problem. VM 5 sometime need up to 5 times longer to compute the toolpath as vm 4 did. Time I do not have.
Often it crashes after or while prozessing. It looks like blocked mamory. Mamory that was in use while generation is not free after the job is done. So VM5 crashes.
at this time I have stopped my testing with VM5, because it is too slow, complicate and buggy at this time. VM 4 does allmoste a very fine job, OK some things are a litle bit tricky and need attention, but it works well.
So I use VM4 and wait for better times.
best regards
Peter
I have the same problem. VM 5 sometime need up to 5 times longer to compute the toolpath as vm 4 did. Time I do not have.
Often it crashes after or while prozessing. It looks like blocked mamory. Mamory that was in use while generation is not free after the job is done. So VM5 crashes.
at this time I have stopped my testing with VM5, because it is too slow, complicate and buggy at this time. VM 4 does allmoste a very fine job, OK some things are a litle bit tricky and need attention, but it works well.
So I use VM4 and wait for better times.
best regards
Peter
Performance ???
Hi gang, hi MecSoft.
Can anyone explain me what "insert cutter" means???
What about inerting the correct filename in the postprocessed file?
VM allways inserts the "VMtempacl.acl" ???
My CNC-mill needs the correct filename in the file.
Yours
Lars
Can anyone explain me what "insert cutter" means???
What about inerting the correct filename in the postprocessed file?
VM allways inserts the "VMtempacl.acl" ???
My CNC-mill needs the correct filename in the file.
Yours
Lars
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Performance ???
Lars,
You can turn on insert cutters in the Flat and the Corner Radius tool dialogs. If you do that VIsualMill will attempt to find areas where the tool will not completely remove material. This algorithm is very compute intensive since it includes material removal simulation as part of this detection. This could slow down performance quite a bit.
Regarding the other performance issues we are actively looking at them and will report once we have some conclusive findings.
Hope this helps.
You can turn on insert cutters in the Flat and the Corner Radius tool dialogs. If you do that VIsualMill will attempt to find areas where the tool will not completely remove material. This algorithm is very compute intensive since it includes material removal simulation as part of this detection. This could slow down performance quite a bit.
Regarding the other performance issues we are actively looking at them and will report once we have some conclusive findings.
Hope this helps.
-
John Loftus
- Posts: 25
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Laguna Beach, CA USA
Performance ???
Lars,
About your correct file name question ... under the Post Process > Post Process Generator do you have the Post File Name set to the proper directory? C:\Program Files\MecSoft Corporation\VisualMill 5.0\Posts (or where ever yours are located?)
You pick your machine under the Post Process Generator and then click edit and go to > General Tab > File Control > Output File Extension ... you can enter the extension you want to save to (NC for example). You can also set the Post Processor Options to show selection in dialog when post-processing.
When I post, I get the Select Post Processor dialog with the last post type already selected. I then click on the browse button to the right of the Output file area and check that the name and extension is correct and going to right directory (set the directory once and it should remember from then on).
BTW, For purchasers of the software, if needed, Mecsoft will customise your post processor to work with your machine so you should be able to get everything dialed in as you want.
Cheers,
John
About your correct file name question ... under the Post Process > Post Process Generator do you have the Post File Name set to the proper directory? C:\Program Files\MecSoft Corporation\VisualMill 5.0\Posts (or where ever yours are located?)
You pick your machine under the Post Process Generator and then click edit and go to > General Tab > File Control > Output File Extension ... you can enter the extension you want to save to (NC for example). You can also set the Post Processor Options to show selection in dialog when post-processing.
When I post, I get the Select Post Processor dialog with the last post type already selected. I then click on the browse button to the right of the Output file area and check that the name and extension is correct and going to right directory (set the directory once and it should remember from then on).
BTW, For purchasers of the software, if needed, Mecsoft will customise your post processor to work with your machine so you should be able to get everything dialed in as you want.
Cheers,
John
Performance ???
John,
when I post my MOPs, I select the postprocessor as you descibed it.
I have to choose between two different post, one for our HSC machine, one for our "convetional" CNC-mill. The conventional CNC need in row one of the program the correct file name,
e.g.:
1 BEGIN PGM 52-004-001-011 MM
2 ;
3 ;
4 ;MOP NAME: Z-Ebenen Schruppen
5 ; ------------------------------------------------------------
6 ; Datei: VMTempAcl.acl
The "52-004-001-011" is the file name I have to insert manually.
When I post, "VMTempAcl.acl" is written by the processor !!!
Any ideas?
Cheers!
Lars
when I post my MOPs, I select the postprocessor as you descibed it.
I have to choose between two different post, one for our HSC machine, one for our "convetional" CNC-mill. The conventional CNC need in row one of the program the correct file name,
e.g.:
1 BEGIN PGM 52-004-001-011 MM
2 ;
3 ;
4 ;MOP NAME: Z-Ebenen Schruppen
5 ; ------------------------------------------------------------
6 ; Datei: VMTempAcl.acl
The "52-004-001-011" is the file name I have to insert manually.
When I post, "VMTempAcl.acl" is written by the processor !!!
Any ideas?
Cheers!
Lars
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Performance ???
Hi Lars,
If you want to output the program name please do the following
1. In the post process->Post processor generator, double click on the file you are using.
2. In the Start/End tab, in the Start section copy and paste
[SEQ_PRECHAR][SEQNUM]; [PARTNUM]
3. In VisualMill, in the first mop, right click and select properties.
4. In the program #, you can type in anything ex: 52-004-001-011 and it will get output in the post.
Best Regards,
MecSoft Support
If you want to output the program name please do the following
1. In the post process->Post processor generator, double click on the file you are using.
2. In the Start/End tab, in the Start section copy and paste
[SEQ_PRECHAR][SEQNUM]; [PARTNUM]
3. In VisualMill, in the first mop, right click and select properties.
4. In the program #, you can type in anything ex: 52-004-001-011 and it will get output in the post.
Best Regards,
MecSoft Support
Performance ???
Hi!
I made the entries in my post as you described.
In fact, the post does not work properly.
The first rows from the compiled MOp:
1 BEGIN PGM 0 MM
2 ;
3 ;
4 ;MOP NAME: 2 1/2 Achsen Taschenbearbeitung
5 ;50039-001-099
6 ;Flachfräser D8/R0.8
7 ; -----------------------------------------------------------------
8 ; Datei: VMTempAcl.acl
9 ; Postprozessor: HeidenHain_BuR_Automatik.spm
10 ; Werkzeug-Nr: 13
11 ; Werkzeug-D: 7.99
12 ; Spindeldrehzahl (S): +8000
13 ; ---------------------------------------------------------------
14 TOOL CALL 13 Z S+8000
...
In Line "0" instead of "0" "50039-001-099" should appear.
Background:
50039 : Customer
-001 : 1. side to mill (counting up)
-001 : MOps (counting up)
I create for every single MOp a postprocessed file. And I have to edit every file to match the file name with the "EGIN PGM ..." line.
I create single files why: in case of a mill break or other "happenings" I only have to correct and transmit one file to the mill. An other reason is that for overnight operation a mill break detect program is inserted after every MOp.
I would be very glad if you have a solution for me...
Best regards!
Lars
I made the entries in my post as you described.
In fact, the post does not work properly.
The first rows from the compiled MOp:
1 BEGIN PGM 0 MM
2 ;
3 ;
4 ;MOP NAME: 2 1/2 Achsen Taschenbearbeitung
5 ;50039-001-099
6 ;Flachfräser D8/R0.8
7 ; -----------------------------------------------------------------
8 ; Datei: VMTempAcl.acl
9 ; Postprozessor: HeidenHain_BuR_Automatik.spm
10 ; Werkzeug-Nr: 13
11 ; Werkzeug-D: 7.99
12 ; Spindeldrehzahl (S): +8000
13 ; ---------------------------------------------------------------
14 TOOL CALL 13 Z S+8000
...
In Line "0" instead of "0" "50039-001-099" should appear.
Background:
50039 : Customer
-001 : 1. side to mill (counting up)
-001 : MOps (counting up)
I create for every single MOp a postprocessed file. And I have to edit every file to match the file name with the "EGIN PGM ..." line.
I create single files why: in case of a mill break or other "happenings" I only have to correct and transmit one file to the mill. An other reason is that for overnight operation a mill break detect program is inserted after every MOp.
I would be very glad if you have a solution for me...
Best regards!
Lars
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Performance ???
Another change in VM 5.0 that might affect performance is the setting called "Part Sampling Resolution". You can find it under Menu -> Preferences -> Tolerances. If you have this setting at Standard, peformance should be exactly the same as VM 4.0. Anything different would decrease performance.
1) This was introduced in VM 5.0 to handle small parts that require high accuracy.
2) Only affects Horizontal Roughing, Horizontal Finishing and Pencil Tracing methods
As a best practice for standard part sizes - 6in(150mm) nominal length and above, use "Standard" setting. For anything smaller than 1 in use the "Fine" setting. For parts in-between use the "Medium" setting.
Hope this helps.
1) This was introduced in VM 5.0 to handle small parts that require high accuracy.
2) Only affects Horizontal Roughing, Horizontal Finishing and Pencil Tracing methods
As a best practice for standard part sizes - 6in(150mm) nominal length and above, use "Standard" setting. For anything smaller than 1 in use the "Fine" setting. For parts in-between use the "Medium" setting.
Hope this helps.