Showing results for 
Search instead for 
Do you mean 
Reply

Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

I have a question for using the Hole_Chamfer_Milling-Operation with a Chamfer_Tool in NX10.0.2.6. If you have a Chamfer_Tool you automatic get 5 trackingpoints. If I want to use the OD_TIP (TIP-Point at small diameter) there is no possibility to remove material. In my oppinion there should be a possibility to bring in the tool deeper than the "Drive Point". In Hole_Milling I can "Extend Path" at "Bottom Offset", but not in Hole_Chamfer_Milling. Doing something wrong? It would be very easy, we could measure the tool at OD_TIP and produce any possible chamfer if this would work.

10 REPLIES

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

Hi Werner,

 

The chamfer milling tool defines 5 automatic tracking points that can be used -by different operation types- to vary the output (output tracking).

 

Only one of the 5 automatic tracking points is specifically defined for drive tracking (OD_CHAMFER). The other tracking points at tip/shoulder could be measured, this one probably not, it is just intended for drive tracking.

 

You can off course define your own drive tracking points to drive your tool along the upper diameter of the chamfer.

 

Thanks,

 

Toon

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

Hello!

 

Do I have to understand that? Why do you say that the points SYS_OD_TIP and SYS_OD_CHAM can not be used as drive-points? The SYS_OD_CHAM really works. If the tool is measured at this point it works. Material will be removed:

 

Also the SYS_OD_SHOULDER works if you need to create a chamfer inside another hole and there is no place to work with another "Drive Point":

 

But we want to meassure the SYS_OP_TIP and we want to work with it. Because of this we need a possibility to bring in the tool deeper than the "Drive Point". Otherwise no material will be removed:

 

It should look like this:

 

Do you understand this?

 

Thanks for help.

 

Werner

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

[ Edited ]

Hi Werner,

 

You may have misinterpret my reply.

 

I didn't write that OD_CHAMFER doesn't work, on the contrary!

 

I wrote : "Only one of the 5 automatic tracking points is specifically defined for drive tracking (OD_CHAMFER)". 

 

What I mean here is that this specific tracking point is intentionally introduced just to have an ootb drive tracking point for chamfer miiling.

 

This doesn't say anything about applicability of the other tracking points, though OD_TIP will not work as you have noticed.

 

The chamfer milling path processor just drives the drive tracking point of the tool along the csink profile as defined by the csink diameter.

 

To have the path according to your last image you currently would have to define a user defined drive tracking point with "Distance" equal to your "Deeper Measure".

 

Thanks,

 

Toon

 

In addition to the above reply where i tried to limit myself to what is currently provided, I would like to mention that you'r desire to have an alternative way to define how to drive the tool (by offset relative to a selected tracking point OR "drive by diameter") is a known enhancement request

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

Hi Toon, thanks for your answer. Is it possible to get the ER-Number? Then I would like to support this ER in GTAC. Thanks a lot. Werner

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

Hi Werner,

 

So far this has been an internally documented enhancement request, i.e. registered internally only. So no GTAC ER yet ...

 

Thanks,

 

Toon

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

jobe, if you submit an ER, please post it here.  I would like to help this one along......too many other CAM systems can accomplish this already.

 

It's 2015 guys......

Proud Member Of The Reality-Based Community.

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

Hi!

 

I've already created an ER:

ER 7473222; Desc: Working with the SYS_OD_TIP tracking point in Hole Chamfer Milling.

 

It's waiting to be supported ;-)

 

Werner

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

A great enhancement for tracking points would be to automatically calculate either diameter or depth based on entering one of the other. Would save some time using trig or drawing the profile of the tool in another file for custom tools.
NX11.0.1

Re: Hole_Chamfer_Milling with Chamfer_Tool in NX10.0.2.6

It's already possible to define a tracking point for a chamfer tool by specifying ONLY the diameter when you switch the "Definition" from "Full" to "By Diameter.

 

Tom van 't Erve

NX CAM development.

Learn online





Solution Information