I have two differant toolpath with to differant problems both are Surface High Speed Hybrid. One is gougeing the drive surface when it is going from cut to cut. I have changed to a full vertical and also change some other settings on that tab and can not get it not to gouge the vertical wall. You would think if that wall was a drive surface it would not gouge it!!!! But NOOOOOOOOOO! The other is machining a flat surface with some pads and radii around the edges. I have a contianment boundery and I tell it to st inside but NOOOOOOOOO it goes outside the containment boundery! I have been with Mastercam since version 7, But I am telling you I am about feed up with it!!!!!
3
High Speed Hybrid
Started by
Todd Mann from Fastech
, Aug 01 2012 06:56 PM
15 replies to this topic
#1
Todd Mann from Fastech
-
- Members
-
- 229 posts
Member
- Location:Greenfield, Ohio
Posted 01 August 2012 - 06:56 PM
#2
Rickster™
-
- Moderators
-
- 12,167 posts
MOBSTERATOR
- Location:Canadada
Posted 01 August 2012 - 08:57 PM
What version are you usiing?
Do you you have a file you can share?
I use these paths constantly.
Do you you have a file you can share?
I use these paths constantly.
#3
Todd Mann from Fastech
-
- Members
-
- 229 posts
Member
- Location:Greenfield, Ohio
Posted 02 August 2012 - 06:26 AM
I am using X6 MU1.
#4
Rickster™
-
- Moderators
-
- 12,167 posts
MOBSTERATOR
- Location:Canadada
Posted 02 August 2012 - 06:40 AM
Not sure if there is a hybrid bug in mu1, but if you can share the file
I could try it in MU2 for you, if you are reluctant to install it.
Mu2 is all bug fixes
It is very stable,much more than mu1
long shot...Try setting all your surface normals the same way and regen
I could try it in MU2 for you, if you are reluctant to install it.
Mu2 is all bug fixes
It is very stable,much more than mu1
long shot...Try setting all your surface normals the same way and regen
#5
peon
-
- Members
-
- 979 posts
Advanced Member
Posted 02 August 2012 - 07:51 AM
As far as your gouges go, go to your Linking Parameters - Leads - Make sure Horizontal Arc Entry and Exit are at 0.0. Any other value in those two boxes will cause a gouge now and then. Values in the Vertical Arc Entry/Exit should be ok. I have seen this bug since the invention of Hybrid and it still pops up in X6MU1. I do not know if it was fixed for MU2.
#6
Turf Toes
-
- Members
-
- 22 posts
Member
- Location:Washington, MO
Posted 02 August 2012 - 04:11 PM
Peon is right about the horizontal arc entry/exit parameters on the linking page. Too much there and you'll find yourself with gouges. But, the gouges on the vertical walls aren't really gouges, their probably the fact that the tool is tracing up those walls to the next cut. To eliminate this, you need to change the percentage of the tool diameter on the Keep tool down within on the Cut parameter page. Too big of a percentage causes the tool to trace up the walls to the next cut. Lower that percentage and the tool drives up and over these walls to the next cut.
#7
Todd Mann from Fastech
-
- Members
-
- 229 posts
Member
- Location:Greenfield, Ohio
Posted 02 August 2012 - 05:21 PM
Thanks everyone for your help.I am going back to some of the older toolpaths to get this part done but I will check it when I get some room to breath.
#8
Brian @ PM Mold
-
- Members
-
- 551 posts
Wannabe Programmer
- Location:Chicagoland, IL
Posted 06 August 2012 - 11:09 AM
I have run into this in MU2. The problem comes out when using the preserve 3D passes. It doesn't like veritcal walls with sharp corners. Tried closed offsets and upper to lower and would get gouges (not always). Cannot recall having issues with 3D passes turned off. Sent to my reseller and they have sent it into QC. I haven't gotten away from the hybrid - just changed my way of using it. It still works great. Use it on almost every electrode I cut.
#9
lukasz24
-
- Members
-
- 5 posts
Newbie
Posted 08 August 2012 - 08:32 PM
Todd Mann @ Curtiss Wright, on 01 August 2012 - 06:56 PM, said:
I have two differant toolpath with to differant problems both are Surface High Speed Hybrid. One is gougeing the drive surface when it is going from cut to cut. I have changed to a full vertical and also change some other settings on that tab and can not get it not to gouge the vertical wall. You would think if that wall was a drive surface it would not gouge it!!!! But NOOOOOOOOOO! The other is machining a flat surface with some pads and radii around the edges. I have a contianment boundery and I tell it to st inside but NOOOOOOOOO it goes outside the containment boundery! I have been with Mastercam since version 7, But I am telling you I am about feed up with it!!!!!
#10
Brian @ PM Mold
-
- Members
-
- 551 posts
Wannabe Programmer
- Location:Chicagoland, IL
Posted 17 August 2012 - 05:27 AM
Came across another model that was gouging with this toolpath. Played with some settings and found out that it looks like the "Keep tool down within" is causing this. I have it set to default at 100% of the tool diameter and it would sometimes gouge (not all the time). By switching it to .010" and forcing the tool to retract the gouge went away. At 100% I would backplot it and in the area that was gouging it was a transition area between cuts.
Hope this helps!
Hope this helps!
#11
Brian @ PM Mold
-
- Members
-
- 551 posts
Wannabe Programmer
- Location:Chicagoland, IL
Posted 17 August 2012 - 09:03 AM
If that doesn't solve it check out your transition parameters. I had it set to tangent ramp - gouge. Went to Ramp - Angle - 30 - gouge. Angle - 20 - gouge. Angle - 10 - no gouge.
Something else to check.
Something else to check.
#12
Rickster™
-
- Moderators
-
- 12,167 posts
MOBSTERATOR
- Location:Canadada
Posted 17 August 2012 - 09:35 AM
I am using hybrid on that job I posted
the large stock model in
It has sharp corners but all wall are 3 degrees
:crossing fingers: while mold is cutting
the large stock model in
It has sharp corners but all wall are 3 degrees
:crossing fingers: while mold is cutting
#13
alancopp
-
- Members
-
- 11 posts
Newbie
- Location:Rockford,IL
Posted 04 April 2013 - 01:48 PM
I am cutting a die cavity and would like to start on the bottom and cut up. Is there a setting that would allow me to do that with Surface High Speed Hybrid toolpath. We have X6 MU2.
#14
Brian @ PM Mold
-
- Members
-
- 551 posts
Wannabe Programmer
- Location:Chicagoland, IL
Posted 04 April 2013 - 03:00 PM
None that I know of. Sorry! Wish I could be of better help!
#15
alancopp
-
- Members
-
- 11 posts
Newbie
- Location:Rockford,IL
Posted 06 April 2013 - 07:41 AM
Brian @ PM Mold, on 04 April 2013 - 03:00 PM, said:
None that I know of. Sorry! Wish I could be of better help!
I was afraid that was the answer.
alancopp, on 04 April 2013 - 01:48 PM, said:
I am cutting a die cavity and would like to start on the bottom and cut up. Is there a setting that would allow me to do that with Surface High Speed Hybrid toolpath. We have X6 MU2.
That would be a good thing to change with X7.
#16
MotorCityMinion
-
- eMC Learning Group
-
- 1,166 posts
Advanced Member
Posted 07 April 2013 - 09:57 AM
Is this tool path ready for the masses? Granted, a fundamental understanding of which tool path to use with a certain type of terrain and knowing what switches control the variables is required to complete a part in a successful manner that produces results which include timeliness, dimensional stability and cosmetic appeal but some of what I’m seeing here is less than satisfactory.
“:crossing fingers: while mold is cutting” Making statements like this to my boss on a one piece jobs is entertaining.
"I have a containment boundary and I tell it to sit inside but NOOOOOOOOO it goes outside the containment boundary!" Man up, this is how they do it in France.
"As far as your gouges go, go to your Linking Parameters - Leads - Make sure Horizontal Arc Entry and Exit are at 0.0. Any other value in those two boxes will cause a gouge now and then." I’d set my op default to 0.0 for this data field then put tape on the monitor over the location of that dialog box.
"The problem comes out when using the preserve 3D passes. It doesn't like vertical walls with sharp corners. Tried closed offsets and upper to lower and would get gouges (not always)." Trying to preserve 3D passes in a 3D tool path, the nerve of some people!
"If that doesn't solve it check out your transition parameters. I had it set to tangent ramp - gouge. Went to Ramp - Angle - 30 - gouge. Angle - 20 - gouge. Angle - 10 - no gouge." Found the sweet spot! Here is another op default to set. Get some more tape.
"But, the gouges on the vertical walls aren't really gouges, their probably the fact that the tool is tracing up those walls to the next cut. To eliminate this, you need to change the percentage of the tool diameter on the Keep tool down within on the Cut parameter page. Too big of a percentage causes the tool to trace up the walls to the next cut. Lower that percentage and the tool drives up and over these walls to the next cut."
I agree with this statement although it is not germane to this tool path. I came across this situation last week while using SF Contour and SF Parallel on the same faces in a curvy progressive die component, CPM4, using a 3.5mm ball and 3.0mm ball. The vertical walls appeared to have chatter in them. The solution was to semi-finish at plus .002 stock and use a slower feed on the semi- finishing tool then switch to a smaller diameter tool for finishing as this allowed for a smother entry into the vertical wall. Only two pieces on this job so I didn’t have the time to narrow it down as I probably could have tried down milling with the smaller tool first. Not enough chip clearance and flute length on the precision OSG finishing tools could have been a factor as well.
“I am cutting a die cavity and would like to start on the bottom and cut up. Is there a setting that would allow me to do that with Surface High Speed Hybrid toolpath.?" “That would be a good thing to change with X7.”
According to a PDF I came across: 3D HST HYBRID. Optimized cut Order. In Mastercam X7, 3D HST Hybrid Toolpaths now include a new Optimize cut order checkbox on the Cut parameters page. This option defines the cut order Mastercam applies to different cutting passes in the toolpath. Now all we need is Optimize Containment boundary , Optimize Horizontal arc lead in , and Optimize Ramp Angle check boxes.
Perhaps some of the new beta testers could comment on this as other changes to the toolpath may be in the works.
“:crossing fingers: while mold is cutting” Making statements like this to my boss on a one piece jobs is entertaining.
"I have a containment boundary and I tell it to sit inside but NOOOOOOOOO it goes outside the containment boundary!" Man up, this is how they do it in France.
"As far as your gouges go, go to your Linking Parameters - Leads - Make sure Horizontal Arc Entry and Exit are at 0.0. Any other value in those two boxes will cause a gouge now and then." I’d set my op default to 0.0 for this data field then put tape on the monitor over the location of that dialog box.
"The problem comes out when using the preserve 3D passes. It doesn't like vertical walls with sharp corners. Tried closed offsets and upper to lower and would get gouges (not always)." Trying to preserve 3D passes in a 3D tool path, the nerve of some people!
"If that doesn't solve it check out your transition parameters. I had it set to tangent ramp - gouge. Went to Ramp - Angle - 30 - gouge. Angle - 20 - gouge. Angle - 10 - no gouge." Found the sweet spot! Here is another op default to set. Get some more tape.
"But, the gouges on the vertical walls aren't really gouges, their probably the fact that the tool is tracing up those walls to the next cut. To eliminate this, you need to change the percentage of the tool diameter on the Keep tool down within on the Cut parameter page. Too big of a percentage causes the tool to trace up the walls to the next cut. Lower that percentage and the tool drives up and over these walls to the next cut."
I agree with this statement although it is not germane to this tool path. I came across this situation last week while using SF Contour and SF Parallel on the same faces in a curvy progressive die component, CPM4, using a 3.5mm ball and 3.0mm ball. The vertical walls appeared to have chatter in them. The solution was to semi-finish at plus .002 stock and use a slower feed on the semi- finishing tool then switch to a smaller diameter tool for finishing as this allowed for a smother entry into the vertical wall. Only two pieces on this job so I didn’t have the time to narrow it down as I probably could have tried down milling with the smaller tool first. Not enough chip clearance and flute length on the precision OSG finishing tools could have been a factor as well.
“I am cutting a die cavity and would like to start on the bottom and cut up. Is there a setting that would allow me to do that with Surface High Speed Hybrid toolpath.?" “That would be a good thing to change with X7.”
According to a PDF I came across: 3D HST HYBRID. Optimized cut Order. In Mastercam X7, 3D HST Hybrid Toolpaths now include a new Optimize cut order checkbox on the Cut parameters page. This option defines the cut order Mastercam applies to different cutting passes in the toolpath. Now all we need is Optimize Containment boundary , Optimize Horizontal arc lead in , and Optimize Ramp Angle check boxes.
Perhaps some of the new beta testers could comment on this as other changes to the toolpath may be in the works.
