Face Milling Offset

[Anonymous]

It would be great to have the ability to offset the face milling operation, EG. using an 80mm face cutter to face 60mm plate, so HSM generates a single tool path on center-line of the part, this was no good for the material or cutter i was machining so I had to manually edit the G-code to offset the Y value, being able to do this is HSM would be much better.

[Steinwerks]

In the Passes tab set the cut width to the diameter of the cutter.

[Anonymous]

@Steinwerks

@Steinwerks cut width?

[Steinwerks]

Sorry wasn't at a computer, set the Stepover to the width of the face mill:

[Anonymous]

@Steinwerks Makes no difference as the cutter is 80mm and the part is 60mm, what I would like to achieve is off set the Y value, currently posting Y0.0 (on center-line) but i want to off set the cutter to Y-10.0 and still on do 1 cut.

[Steinwerks]

Ah, that was not clear. Are you tied to using Face to do this? It can be a 2D Contour very easily in this example.

[Anonymous]

@Steinwerks, for my part above I would need to sketch a path for 2D contour as I can not select a line the length of the part very easy, and would that not defeat the purpose of having a facing cycle to use?

[Steinwerks]

If you turn on Stock Contours with no selection it should extend past the stock no matter how long the contour you select is.

I'm not saying your idea isn't valid, but Face is probably one of the least-smart and least-developed toolpaths in HSM and I wouldn't expect many changes. Just trying to give you a repeatable workaround that won't require you to edit the code manually.

[Anonymous]

@Steinwerks just tried that and no selection would not let me, it wants a contour selected. fully understand and appreciate the help, this has been the only time where the facing cycle has let me down, and it was only because of the type of material and the intermittent cutting that the offset was needed, and even with the offset we still indexed the tips after each part, but the offset did help in the load on the machine and the sound of cutting.

[Steinwerks]

@Anonymous

I just tried this in Inventor and got this: 

You still have to select a 2D Contour, check the Stock Contours box but do not enter any Stock selections.

[Anonymous]

@Steinwerks thanks for that, I just had a play and ran it in Sim, by doing the contour the tool will follow that edge, which means the edge of your part will be the edge of the tool, so to get the face cutter over the edge a sketched path is still needed? unless i am missing a way to off set the contour path?

[Steinwerks]

Use a negative value for a Radial Stock to Leave setting.

[Anonymous]

@Steinwerks cheers for all the help and work around.......i still stand by the idea though as thats alot of mouse clicks and mess abouts with things to remember for something as simple as adding a offset value in the UI haha

[Laurens-3DTechDraw]

I'm actually all for the way the software handles it now. If I can do it in one pass I tend to want it in the middle.

But I understand the request but see no way of making it in the UI in a way it's only there when the cutter has to do one pass.

[Anonymous]

@Laurens-3DTechDraw until this job i was happy with how the software worked in regards to the facing also, but with out the offset the cutter is effectively conventional cutting the 1st half of the arc and climb cutting the 2nd half of the arc, by off setting the cutter it is only climb cutting, and when going over top of the part in my photos it makes a huge difference due to the intermittent cutting, surly just adding a offset value box in the UI would work? it would not mater if there was a offset even if it was not on center, but the user would only input a value when they required an offset otherwise the default would be 0mm?

[al.whatmough]

Batch processing ideas that are 10+ months old with less than 5 votes. This is in no way to suggest the idea isn't a good one. However, the lack of votes tends to mean that the community feels other ideas should be given a higher priority. Feel free to tag me if you feel an idea wasn't given enough of a chance. We are more than happy to have a conversation on any of these ideas.

[Anonymous]

Hi

I want to ask, is there any possibility to implement any offset to single pass milling?

I have the same problem, when I want to face-mill a narrow workpiece with a wider milling head.

In Sandvik machining guide i found that the cutter should be off-center.

Why does software don't do that automatically, like in multipath situations?

This change would improve surface quality and increase tool life.

Facing can be done by 2D Adaptive or contour, but only in Face there is a "chip thinning".

Also are you planing to implement "chip thinning" to other strategies, like 2D Adaptive or 2D Pocket?

It is a grat technique, it increases tool life and it is faster than entering straight to the material.

It is a pity that this technique is only available in Facing, where milling heads are also used in other strategies.