Looking for 4th axis help.

[bmadsen]

Pro Engineer users,

I've been working on the slots on the cam tube in this photo for quite some time now and I'm getting fed up with Pro-E. I feel like I've tried everything.

Here's my situation: I'm machining this tube all at once in a Mazak Integrex with 5 axis and live tooling. However the controller is only set up to move 4 axis on the machine at a time instead of 5 axis. The full 5 axis capabilities is another $20k so the company I work for decided against that. As far as the cut goes. The engineer drew the part so that the walls of the slots are completely aligned with the center axis of the tube. I'm using Creo 1.0 and the best way to get a tool path on the part has been 4th axis trajectory milling or 4th axis surface milling. The trajectory milling using the axis control looks liked it worked at first but looking at it closer the tool axis of the end mill was not following the geometry due to the tool Y axis of the machine not pointed at the center of the tube. Why is Creo moving the Y axis of the machine when all that needs to move is the X, Z and C axis?

And then you would think that since surface milling rotation can point at the center axis of the tube that should work great. Wrong. It has been very difficult to even create a tool path. Creo says it can't create a tool path because of gouging. Why can't Creo tell you what to fix in order for it to work? And why can you draw the part in Pro-E but it can't machine it?

I really wish Pro E would go through and test every different possibility and fix the bugs on the Manufacturing side. It could be so much better.

Any help would be appreciated.

Thanks,

Brian

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[bmadsen]

Creo users,

If you look at the slide show attachment sent by Terry you will see that in one photo the tool axis is parallel with the surface creating the tool axis to be off center. And in the other photo the tool axis is pointed at the center of the part but it will not cut the surface correctly. My coworkers and I thought the tool axis should be pointing at the center of the part. But we now understand that the tool axis must be parallel to the surface it's cutting. And the only way to achieve this is to use simultaneous 5 axis milling (which we don't have activated on our Integrex). What we're going to do is cut as much as we can on the lathe and then cut the slots in our Mazak VTC-800 using a rotary table.

I just thought I'd let you know what I came up with. I'm very surprised and grateful for the feedback.

Thank you,
Brian

[rrich]

Brian,
There are some things you can do to force what you want. I would use the 5 axis trajectory milling with tool axis control, thus forcing the axis to be exactly the angle you wish it to be. You will need an axis created fixed to the direction you wish to maintain. The axis does not need to be on the curve or even near were you are machining it just needs to be in your model. Then you will be following a curve that you created, at each transition point you will want to force your tool angle to be at the axis you created. You can then tell the feature to ignore the part so that gouging error would go away. Then your post must deal with the code they way you want. My guess is you could leave it as a 5 axis post and your machine will only deal with the proper code for 4 axis and ignore the rest.

It has been a while since I have done this and do not have access to the CNC module any longer so I cannot give you a sample at this time. Last time I messed with it was in WF4, so things could be different at this time.

Ron

[TomU]

Is there any way you could create a curve right down the middle of the slot and then use trajectory milling to simply follow that curve? You would need to turn off gouge checking, but at least the cutter would go where you want (and spit out the G-code to do so.)

Tom U.