[lovemygirl]

I have a sketch...in one image with the tool...and I have the IGS file olso...can somebody help me??? maybe with some ideas. I don't have a simultaneous 5 axis machine. thanks

[txcncman]

Can't be done on a 3 or 4 axis machine without special fixturing/sine plate.

[lovemygirl]

Can't be done on a 3 or 4 axis machine without special fixturing/sine plate.

I have everything...but I don't know how to make the program in mastercam....maibe I have to create one machine definition...but with a rotary axis at 33 degrees....or something....Can I do this...how can I change the rorary axis in mastercam...can I chose one arbitrary axis???

[etech4u]

I think the only way this could be done in mastercam is using a lollipop cutter and programming it fully 5axis. That is how we would do it at my shop. I think before we went to that time and expense of figuring it out I would ask the customer if he knew what he was designing. The part seems a bit odd to me.

[Ydna]

If you have a 4th axis indexer that bolts onto the table, you might be able to position it up at an angle (33?) in order to access that groove. You'll have to make a special wedge for the indexer and it might have to be programmed using mastercam's 5 axis module. I can't say myself since I've never done a part like that in mastercam.

I've made parts like that before but they had less complicated geometry...yeesh

[lovemygirl]

thank you all

[Superman]

I have everything...but I don't know how to make the program in mastercam....maibe I have to create one machine definition...but with a rotary axis at 33 degrees....or something....Can I do this...how can I change the rorary axis in mastercam...can I chose one arbitrary axis???

OK, it can be done with a standard 4 axis post.

Select your CNC machine as per normal, then "Edit" the control definition, using the Edit button that is in the operation manager....this is to modifiy this session only, it does not modify the CNC machine or the control that you have already proven as OK. If you reload this CNC machine again, you will lose your setup mods

For the Control description
When editing the control, you need to modify what angle your 4th axis is set at, relative to your programming

For the toolpath
WCS is the actual setup with the 4th angle tilted at 33°, The T/C planes is the view down along the tool axis toward the part, where the tool is to start cutting.
--- You may have to enable Rotary machining ( around A ) ( haven't done it for a while )
--- you expect that the output (for actual machining ) is to consist of X, A, and Z movements

( you may get a Y movement only when a straight section is encountered )

[lovemygirl]

OK, it can be done with a standard 4 axis post.

Select your CNC machine as per normal, then "Edit" the control definition, using the Edit button that is in the operation manager....this is to modifiy this session only, it does not modify the CNC machine or the control that you have already proven as OK. If you reload this CNC machine again, you will lose your setup mods

For the Control description
When editing the control, you need to modify what angle your 4th axis is set at, relative to your programming

For the toolpath
WCS is the actual setup with the 4th angle tilted at 33°, The T/C planes is the view down along the tool axis toward the part, where the tool is to start cutting.
--- You may have to enable Rotary machining ( around A ) ( haven't done it for a while )
--- you expect that the output (for actual machining ) is to consist of X, A, and Z movements

( you may get a Y movement only when a straight section is encountered )

...So I chose General Haas 4 axis vcm....in the Machine Definition...right click on A axis I chose properties and I make the the changes ..Tilt Angle I chose the tilt about Y axis and a put my angle??? It's ok like this?? and the angle it would be 180-33 in CCW positive. In the Defined angle(from 0 deg.) I put something or I leave the field like it is??

And in the Dynamic WCS----I make the X axis pointed in the directon of the tilt angle? or my WCS it will be normal...only the 4axis it will be different???

I understand something or make fun of me ??

Thank you very much and a Happy New Year.

[Superman]

So I chose General Haas 4 axis vcm....in the Machine Definition...right click on A axis I chose properties and I make the the changes ..Tilt Angle I chose the tilt about Y axis and a put my angle??? It's ok like this?? and the angle it would be 180-33 in CCW positive. In the Defined angle(from 0 deg.) I put something or I leave the field like it is??

NO...do not use the "settings" pull-down on the upper toolbar, stay away from the machine definition area...you are making permanent changes to your everyday CNC machine
---use the "Edit" button in the operation manager ( "Files" tab ), to only modify the CONTROL definition for this program setup. If you reload the CNC machine file, then any mods are deleted.

To get your tool into the area ( as per your drawings ) the A axis has to be on it's back (pointing up ) and then tipped 33° CCW...the angle to be put into the A axis tilt is 303° (360-57)


And in the Dynamic WCS----I make the X axis pointed in the directon of the tilt angle? or my WCS it will be normal...only the 4axis it will be different???

The WCS ( X axis ) will be perpendicular the the axis of the tool ( shown in your 2nd drawing ) .
Looking from the TOP, X will be along the A-axis
Looking from the FRONT, X axis will be rotated 57° CCW from the system's X-axis

I understand something or make fun of me ??
?? not sure what you mean by this comment :tired::nono:


etech4u pointed out that this design may be flawed, this undercut cannot serve any purpose... part isn't round, so this area doesn't move against anything else...it appears to be a "handgrip" of some sort.
- a design change may turn it into 2 peices, a disc withe a spigot with this O'ring groove, and a "handle" that is bolted onto the spigot...or replace this undercut with just a fillet


PS....I did notice drawings were done in Delcam. Any reason why it wasn't done on Powermill ??

[lovemygirl]

So I chose General Haas 4 axis vcm....in the Machine Definition...right click on A axis I chose properties and I make the the changes ..Tilt Angle I chose the tilt about Y axis and a put my angle??? It's ok like this?? and the angle it would be 180-33 in CCW positive. In the Defined angle(from 0 deg.) I put something or I leave the field like it is??

NO...do not use the "settings" pull-down on the upper toolbar, stay away from the machine definition area...you are making permanent changes to your everyday CNC machine
---use the "Edit" button in the operation manager ( "Files" tab ), to only modify the CONTROL definition for this program setup. If you reload the CNC machine file, then any mods are deleted.

To get your tool into the area ( as per your drawings ) the A axis has to be on it's back (pointing up ) and then tipped 33° CCW...the angle to be put into the A axis tilt is 303° (360-57)


And in the Dynamic WCS----I make the X axis pointed in the directon of the tilt angle? or my WCS it will be normal...only the 4axis it will be different???

The WCS ( X axis ) will be perpendicular the the axis of the tool ( shown in your 2nd drawing ) .
Looking from the TOP, X will be along the A-axis
Looking from the FRONT, X axis will be rotated 57° CCW from the system's X-axis

I understand something or make fun of me ??
?? not sure what you mean by this comment :tired::nono:


etech4u pointed out that this design may be flawed, this undercut cannot serve any purpose... part isn't round, so this area doesn't move against anything else...it appears to be a "handgrip" of some sort.
- a design change may turn it into 2 peices, a disc withe a spigot with this O'ring groove, and a "handle" that is bolted onto the spigot...or replace this undercut with just a fillet


PS....I did notice drawings were done in Delcam. Any reason why it wasn't done on Powermill ??

Thank you for your time Superman....I do not speak english every day...so maybe I write something meaningless..sorry about that.

Yes I understand about Machine definition...edit it from Operation Manager..I will not use the "settings" pull-down,on the upper toolbar.

I have powermill olso...but like in mastercam I'm new in 4-5 axis.

Thank you..I will try to see what happens.

[Hedelius]

I have a sketch...in one image with the tool...and I have the IGS file olso...can somebody help me??? maybe with some ideas. I don't have a simultaneous 5 axis machine. thanks

Fancy bottom plate, hahh?