mcpgmr
-
Posts
761 -
Joined
-
Last visited
Content Type
Profiles
Forums
Downloads
Store
eMastercam Wiki
Blogs
Gallery
Events
Posts posted by mcpgmr
-
-
To anyone interested. The solution we came up with is just simply updating WCS for each feature on the part. I reset all WCS's that were updated and all of the extended work offsets back to match G54 values at the end of the program using a sub call. G54 on these machine never changes since it's at the trunnion rotation point. Productivity + is pretty cool and powerful if used properly.
O7200 (RESET WCS VALUES TO MATCH G54)
G00 G90 G54
G10 L2 P1 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L2 P2 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L2 P3 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L2 P4 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L2 P5 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L2 P6 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L20 P1 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L20 P2 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L20 P3 X-12.4016Y-23.6221Z-25.5905A0.C0.
G10 L20 P4 X-12.4016Y-23.6221Z-25.5905A0.C0.
M99 -
13 hours ago, cncappsjames said:
That would most likely require some pretty heavy Post Processor mods with buffers but sounds possible.
@Colin Gilchrist may be able to provide some specifics as to how to achieve it.
Thanks James. I reached out to Collin last week but at the time he was just too busy to look at it. I have my reseller working on alternative methods. I may be able to use G10 to update the wcs for each plane. I tried using G55-G59 and G54.1 P1, p2 etc.. also. The post was set to lock on the first wcs used which results in G54.4 P1 only but when I unlock it I get multiple dynamic offsets out of the machines range along with G55-G59 and G54.1 P1, P2 etc...
This post is for a Mazak Variax i700 Matrix and Smooth controllers. It's probably 8 years old and I may need to get a new post written. I am barely a post guy. I can tweak thinks and force things but this stuff is way over my head.
Thank for you time sir!
-
1
-
-
19 hours ago, cncappsjames said:
That should work. Are you wanting the post to add in the #601, #602, etc... automatically?
Good morning,
Yes I would like to use the values from #601 to #610 that were recorded by Prod+ to be out put like the example code that I posted. I have 9 holes I need to countersink each from a different plane. The part surface varies from part to part and from hole to hole. Lets call it a wavy surface that meets profile tolerance but the countersink diameters will not stay in tolerance because the countersinks dia tolerance is +/-.005 The following example works but is hand written to do so. The countersink depth to achieve the Ø.405 +/-.005 is Z-.17 Example: G98 G82 Z[#603-.17] R4.4782 F6.79 P3000.
-
Good morning,
I would like to know if anyone has had any experience with using a variable that was set by the Prod + to change a tool length wear offset. Example, Probing in 3+2 on our Mazak i700 Matrix and smooth controllers. I'm setting variables #601 through #610 to store the Z values at hole locations on a complex airflow surface on a CFRP part. These parts vary from one to the next and I have to probe every part at every hole location so that I can maintain Ø.405 x 100 ° countersink at each hole location. I have +/-.005" on the diameter and the parts vary more than that in most cases. Up until recently these probing routines were written by hand and work very well. We don't want to do that anymore and would like Prod+ to do it for us. here is a sample of one of the programs that works for us.
T101 M06
T102
G00 G90 G54
S679 M03
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-96.6726 C-5.9027
G54.4 P1
A-96.6726 C-5.9027
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X-2.0726 Y-5.9714 M08
G43 H101 Z8.5289 M51
G98 G82 Z[#601-.17] R5.1289 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0.(COUNTERSINK PER DWG HOLE 2)
G00 G90
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-90.3464 C36.2665
G54.4 P1
A-90.3464 C36.2665
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X4.255 Y-5.1699
G43 H101 Z8.2982
G98 G82 Z[#602-.17] R4.8982 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0.(COUNTERSINK PER DWG HOLE 3)
G00 G90
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-89.0061 C43.1306
G54.4 P1
A-89.0061 C43.1306
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X5.4498 Y-7.2461
G43 H101 Z6.3782
G98 G82 Z[#603-.17] R4.4782 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0.Thanks in advance!
-
Correction to dropbox link.
This is a video capture of Vericut running.
-
I have attached a link to my dropbox. This will give a better idea of what I'm doing if anyone is interested.
-
2 hours ago, Miki67 said:
Are you using Productivity + to output to #601
or you wanted to know how to do it
I have probed all of the hole locations (3+2) positioning and can store those values in #601 to #609. I've done this before I drilled the holes. Now after the holes have been drilled I would like to countersink the holes using their respective values stored in the variables to incrementally countersink each hole from the part surface. This would be easier if it was not 3+2 positioning. I have to probe at the hole center line and normal to the surface. There is a barrel screw at each hole that I am reaching through to access the part surface. I'll check to see if I'm allowed to share a screen shot.
-
That's correct. The example I've given was written by hand. What I'm looking for is a method to get the same output or result from Productivity +.
Just now, mcpgmr said:That's correct. The example I've given was written by hand. What I'm looking for is a method to get the same output or result from Productivity +.
28 minutes ago, Jake L said:If I'm reading this correctly, it looks like your Z value is the value stored in #601 minus .17. So this code should machine a Ø.405 csink.
To change the csink dia just change the .17 value to the depth you want the csink tool to go below the surface.
-
Good morning,
It's been a long time since I posted here. I hope all is well with everyone I used to know here and those of you I haven't interacted with. I'm starting to implement Productivity + and would like to know if anyone is using the software within MC 2022. Up until recently one guy used to hand write the probing routines and he is no longer with the company. I have used P+ for some pretty basic stuff and have been successful but now I want to get fancy with it and am looking for some guidance. I took part in the training about a year ago and really didn't get a lot from because we didn't jump in and start using it right away. I'm working on a complex compound air flow surface drilling and countersinking CFRP parts that require a 100 deg countersink that has a diameter dimension of +/-.005. The surface of the part I'm countersinking has some variability due to the nature of the CFRP material. I want to probe at the center line of the holes normal to the surface and store the information from each hole surface to a variable before I drill the hole. Then before I countersink I would like to use the information stored to countersink incrementally from the Z location stored for each hole surface. So far I probed all hole locations and stored the Z surface point values to #601 to #610. Now I need some direction on what to do next in order to accurately countersink and maintain the +/-.005 countersink diameter. Below is an example of the hand written code that was used to do this on other similar parts we machine. Any help would be greatly appreciated. Thank you!
N2
(COUNTERSINK PER DWG HOLE 1)
(T101 - 9/16 COUNTERSINK 100 DEGREE - H101 - D101 - DIA .5625")
T101 M06
T102
G00 G90 G54
S679 M03
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-96.6726 C-5.9027
G54.4 P1
A-96.6726 C-5.9027
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X-2.0726 Y-5.9714 M08
G43 H101 Z8.5289 M51
G98 G82 Z[#601-.17] R5.1289 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0.(COUNTERSINK PER DWG HOLE 2)
G00 G90
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-90.3464 C36.2665
G54.4 P1
A-90.3464 C36.2665
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X4.255 Y-5.1699
G43 H101 Z8.2982
G98 G82 Z[#602-.17] R4.8982 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0.(COUNTERSINK PER DWG HOLE 3)
G00 G90
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-89.0061 C43.1306
G54.4 P1
A-89.0061 C43.1306
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X5.4498 Y-7.2461
G43 H101 Z6.3782
G98 G82 Z[#603-.17] R4.4782 F6.79 P3000
G80
G54.4 P0
G91 G28 Z0. -
Thanks Colin. Turns out the kinematics were set wrong for our machine from the reseller in the RenMF file. I figured out. Still haven't heard back from Renishaw. All is good now though. Thanks for taking the time to reply.
-
1
-
-
Hi Collin,
While I'm waiting 4 days now for both my reseller and Renishaw to get back to me on a problem I'm having, I was wondering if you might have some insight. I'm 3+2 probing a surface on a fixture. The "A' and "C" angles output from Prod+ do not match if I drill at the same point using the same plane as the probe. Actually the "A" axis is correct but the "C" Axis is way off. Using Mastecam 2022 and programming for a Mazak Variax i700 with the Smooth control. The probing works fine for 3 axis. I've tried adjusting the kinematics settings in the RenMF editor without any luck. Any ideas what could be going wrong? Any help would be much appreciated.
Thank you!
-
1 hour ago, jeff said:
That must be one hell of a groove if it has a 1 hour run time! Can you share a picture?
No sorry I can't share. One off part that we had no time to buy the proper face grooving tool.
-
Anyone use Tool Inspection function in the grooving operation? MC 2019 Lathe. I have a grooving operation that runs for an hour and would like to have the tool retract and the machine stop to inspect the tool periodically. Turned it on and set the parameters to my liking and it has no effect on the code when I re-post. Perhaps the post doesn't support it? I've poked around in the post and don't see any references to Tool Inspection. Post is for a Puma 2600SY dual spindle lathe. About 5 years old. Any input would be appreciated.
Thanks in advance.
-
Doing well thanks how are you? Coming up on 10 years here now. Got separated 3 years ago. That was rough but bounced back.
.gif ":)")
Enjoying my Harley and my girl friend that also enjoys my Harley. Life is good! 
-
2
-
-
Hello fellow programmers. Good to see the site still going strong. I pop in now and again but never long enough to hang out and read much. Hope you all are doing well.
Paul
-
1
-
-
34 minutes ago, CEMENTHEAD said:
I use Cobalt end mills (razor sharp & ease of regrinding), slow speeds to keep the dust down. no coolant, although you could use distilled water but not if you want to hold any close tolerance (due to absorption). we use a light air blow into a vac.
If possible try and keep the cut / chip direction always spinning into the part as it would chip if you pull a chip off the edges.
SFM ? RPM? Was going to use 60 SFM which is what's recommended for graphite machining. Also was going to use a carbide 1/2"ball e.m. Helical milling holes through 1" plate. Holes are Ø.515 and Ø.750
-
Hello,
Any Speed and Feed recommendations? Carbide, diamond coated end mills?
-
:bump:
-
-
Well we found a bandaid for this that helps. Once the operations are assembled, Edit the parameters of the first child operation and turn on transitions and set the lead in/out and the overlap. Then regenerate that op. Right click on the parameters of that op and drag it to the next op. Easier then opening each op up and turning on transitions etc... Do that to each operation and regenerate them when finished. Only downside to this method is that if you change the paren operation then it recreates all the child operations and you have to go back in and repeat the process that I just explained.
-
Thanks, I sent you the file. I'm also sending it to my reseller Prism Engineering.
-
Yes, X7 MU2. If I sent you the file would you mind taking a look at it?
-
bogusmill,
Drill 5axis would have been perfect for that. You just have to create points and use your surface as a guide to automatically create the vectors for you assuming all your holes are on one surface. Or you could use Solids/Hole-Axis to create the vectors and points and uses the lines and points options to control the tool axis.
This is what I have been using up until now.
-
Definitely has Bugs in X7. It's FUBAR no matter what I do. Conventional, Climb, Start from center you name it. I might trust it for drilling but that's it!
Productivity + question
in Industrial Forum
Posted
I like it! Thank you sir! I will have to convince the operator who is very resistant to change that this would cover our butts if G54 would ever change. Thanks again!