45 degree angled head

[peon]

We just purchased a 45 degree angled head to attach to our VMC's. We want to use surfacing toolpaths and this head for machining detail in our molds. Where do I start with this contraption? Do I make a new machine definition? Must I use a router post? I don't have the 5 axis license and not sure if I can really use this new toy.

[peon]

bump

[mayday]

Fixed head? aligned in the X or Y axis?

 

you may have to set up a aggregat head. There is a C-hook for that I think but never used it.

Cant tip the part at 45 degree's ?

[Bruce Kanzelmeyer]

I think you should be able to define 45 degree planes in your View Manager and then go to town using your standard 3 axis toolpaths. In the Planes tab in your operation dialogue box leave the Working Coordinate System as Top and select your 45 degree planes as the Tool and Construction Planes. I also set the XYZ values of the plane(s) origin to 0,0,0 so that its the same as the WCS for your standard 3-axis toolpaths. I'm not sure what the best way for you to define your tool length is, though--I use this method to drill holes or rout contours at unusual angles with my 5-axis router and I know exactly what my pivot distance is to set my tool length. You'll have to figure out what that is for your gear.

[peon]

I was hoping to tip the part at 45°, but the part is too big. The head will be setup and fixed with the tool pointing to X+. Bruce, that all makes sense to me but I have a question about the tool length. Is it best to have the tool setup in the head and then take the measurement?

[Bruce Kanzelmeyer]

Not sure. Do you have a tool setter or probe system on your machine? Imagine that the tool is vertical, and touches off tool setter, and then rotates up to 45 degrees. You need to know what that "pivot" distance is--the length from the tip of tool to the pivot point on the head. Did the 45 degree head manufacturer give you any info on this? Maybe it's just a matter of doing some trig--if you're using standard EM, just offset radius at 45 degrees to set length. Bullnose cutters offer additional challenges, but ballmills are easier!

[peon]

I do have some data to sort thru, but just got buried by a quick hot project. I do have the tool backplotting correctly, but I can't get the solid component (angled head) attached to the tool. In the help file, it mentions I must add a router spindle to my machine def. This is where I'm getting lost for the time being. I need to see that angled head attached to the tool during backplot or verify since it will be machining in a large cavity.

[Tyler Robertson]

if I understand you correctly, I think you're going to need to use machine sim for that\

 

the backplot will show your spindle at whatever angle, but it spins a conical shape for the tool for backplotting, so your angle head solid if you do attach it, will be spun around the tool. Unless I'm missing something

[peon]

Ah, I was wondering about that Tyler. I'll keep playing with it.

[GoetzInd]

Maybe Robk will chime in. He has done some pretty cool stuff with angle heads. I'm sure he's got it figured out.

 

Mike

[Tyler Robertson]

the help in machine sim does a decent job of explaining how to add a solid to a machine - you don't have to have a machine indentical to yours if all you really care about is the 45 degree head, otherwise you'll want to get or draw cad for your machine

[Colin Gilchrist]

You will need to use a Router Post for this to work. The Router Posts have special logic for handling the Aggregate head parameters.

 

(If necessary, you can contact your Reseller for a document that describes how to convert a Router Post into a Mill Post. This will let you run the Router Post with the Mill Product).

 

All Router Posts are built as 4X Posts, with the Rotary Axis mounted on the Z Spindle. This means you will not be able to post a 4 axis toolpath, unless your aggregate is a full rotary, as the Router Post is configured to control a 'C' axis, that rotates about Z.

 

You will need to edit your Machine Definition and add an Aggregate Head component. In the Aggregate Head Parameters, you'll need to select "Compound Angle" as the aggregate type.

 

Set the Orientation to "Fixed".

 

Imagine looking down at your part from the Spindle. Is the tool pointing towards X+ (Angled towards the right)? If so, your Machine View Angle will be 0.0 degrees. (If that is backwards, just enter 180). Next, enter 45 degrees in the Tilt Angle parameter. The last parameter is 'Tool Axis Length' and this number should be your gage length from the pivot point of the head, to the gage line of the tool holder. (The X offset, Y offset, and Z offset are not used by default in the Mill or Router Posts. They are available to a Post writer, but do not change the NC code unless they are hooked up)

 

After you have setup the Aggregate parameters, Right click on the station, and add a tool. (either from the library or create a new tool definition). The overall tool length number will be added to the 'Tool Axis Length' parameter when you post. (there are switches in the Router Post that control how the code is calculated).

 

Do NOT turn on this setting in the Control Definition: On the Work System page, turn on the 'Translate NCI coordinates to Machine View with Aggregate'. The Post handles the offsetting of the NC code.

 

When you are programming for this aggregate, you'll need to measure your tool length as it has been setup on the machine, and enter those values into Mastercam. If you have to adjust the cutting on the machine, you'll need to edit the tool length in Mastercam and re-post your NC code.

 

There are a couple variables in the Router Post that determine how the coordinates are calculated, and control if the Post uses the OAL value of the tool. I'd strongly recommend contacting your reseller for help on setting this up if possible.

 

Hope that helps,

[peon]

Thank you for explaining that very well Colin!! I will get as much setup as I can and call my reseller on Monday.

[robk]

I would cut a 45° slot on the fixture with known dimensions. You could then touch off your tool to the slot and do some trig to figure out your length and stickout. This is not something that I do, but just something that I envision in my head and it should work.

Our situations are a little different because we use 90° heads and use tooling balls on our 3+2 horizontals. On the Integrex style machines I have the operators use the tool eye to set the lengths/stickouts. Then tilt the RAH at any angle to machine the part. In my programs I use coordinate system rotation (G68) on our head-table machines. G68 should work in your case also without doing the "physical" roation. I don't have any tips for you with programming/posting because I do not use mastercam.

[peon]

Well, I contacted our reseller. They aren't able to help me. They sent me some documentation regarding posts, but in those docs, it only shows you how to convert a mill post to a router, not vice versa. They are going to get a quote from In-House Solutions to get me what I need. I didn't think I should have to pay for something like this. I just want to use the aggregated head. My coworker toolpaths in Pro/e and he just had to create a 45° plane and add some numbers for that head and was done. He didn't need a separate post, but just a phone call to Pro/e. I was shocked it was that easy for him. Not to mention, his package includes Vericut, which accurately displays the entire head, tool and workpiece. I'll contact CNC directly after I get the quote from my reseller and hopefully they can help.

[mkd]

+1 for Colin's explanation.

 

i would get the 5 axis license, as there are a few ways to do this. a five axis post will likely have the ability to read Misc Values for the angle of the head.

 

as another method, you can setup a tooling ball at a known location, which would be instrumental to getting the centerline and tool tip setup with machine offsets or g92 method. i just recently did some five axis holes on a 3 axis machine this way (dual angle head of course). used a head-head post with zero for tool length. worked like a charm.. and passed inspection.

i've also done this for a right angle head on a full 5 axis machine and swarf cuts. just had to tweak a trunnion post.

[Tyler Robertson]

Well, I contacted our reseller. They aren't able to help me. They sent me some documentation regarding posts, but in those docs, it only shows you how to convert a mill post to a router, not vice versa. They are going to get a quote from In-House Solutions to get me what I need. I didn't think I should have to pay for something like this. I just want to use the aggregated head. My coworker toolpaths in Pro/e and he just had to create a 45° plane and add some numbers for that head and was done. He didn't need a separate post, but just a phone call to Pro/e. I was shocked it was that easy for him. Not to mention, his package includes Vericut, which accurately displays the entire head, tool and workpiece. I'll contact CNC directly after I get the quote from my reseller and hopefully they can help.

 

Not looking to get into price structure - but I don't think that comparison is straight forward - when you say 'not to mention, his package includes vericut' ... that package would then be significantly more expensive.

if you had a post that supported the head from the get-go, then you would just have to create a 45 degree plane, and add some numbers.

his pro-e package, considering it came with vericut may have had a more complicated post set up with it as well.

[peon]

It is a very FAIR comparison. He contacted his reseller and within a 15 minute conversation they had his software crunching and posting good code (not including the vericut). I call the reseller and get nothing but a future quote.

[Tyler Robertson]

If someone bought level 1 mastercam, and someone else bought level 3 mastercam, and we were talking about 3-d surface machining - the person with level 3 would be up and going within minutes and the person with level 1 would get an upgrade quote.

[peon]

Ah, I understand you now Tyler. See below for a snippet of the resellers Maintenance program ad. It does mention having to pay extra for some 4/5 axis post support, but I would think Mill Level 3 with solids and paying for maintenance would get me some support.

 

 

Ongoing Support

 

Only those customers on maintenance will receive ongoing support from our highly trained, experienced veteran Applications Engineers. XXXXX’s seventeen years as the leading CAM software provider to manufacturers’ means you continue to get the best service and support in the industry.

 

Post Processors

 

Post Processor support is included with your maintenance. Xxxxx has post processors available for over 5,000 machine tools. New piece of equipment? Call us for a working post processor to quickly and easily integrate it into your operations. As a maintenance customer you get access to our Post Processor Library available from our Post Department. Some machines and 4/5 axis posts will require additional charges.

[GoetzInd]

Peon,

Don't you know that maintenance only covers the most basic of post processors?

 

Mike

[peon]

Peon,

Don't you know that maintenance only covers the most basic of post processors?

 

Mike

 

Must be the ones already supplied with the main package. Hahaha. Honestly, my reseller had an individual whom was outstanding at this kind of stuff. He is no longer there. I think the other guys are working hard to pick up his work. I have no issues with the individual helping me now. I'm grateful he's pointing me in the right direction rather than biting on something he can't chew. I don't understand why it is the resellers sole responsibility when configuring this kind of stuff. Shouldn't CNC help the reseller with this rather than relying on another reseller?

[Watcher]

his pro-e package, considering it came with vericut may have had a more complicated post set up with it as well.

 

Well, being a skilled Pro/NC dude and a mediocre GPOST developer I can answer this one with a high degree of accuracy:

 

In fact, RAH support in Pro/NC is just awesome when compared to all softwares I know. Even NX is a joke in this field when compared to Pro/NC.

 

It's not a complicated post setup, but rather, a functionality designed to be straightforward and reliable. It's not a workaround or a post-trick. It's native functionality a click away. The way PTC implemented it (François Lamy) helps the programmer to forget any specifics or abstractions in other softwares...

 

This is what you've got to do in the post to activate it:

 

 

I'd like to say though that in Pro/NC / GPOST this is very straightforward process if you use a 90 degrees AH. You just need to tick a checkbox and construct your Angle Head model using Pro/E rules.

 

A 45 degrees AH would require some coding in FIL language (The equivalent of MP Language in GPOST) to make the right conversions. Not big deal though for an average post writer. You can even find the code on Internet and include it on your post.

 

In regards Vericut integration, the programmer does not have to setup a thing as well because the interface transfer all tool holders, angle heads and fixtures to Vericut automatically. Of couse the programmer still have to push the "Play" button to start the verification...

 

All jokes aside... the standard Vericut interface provided by PTC is good but not perfect. Every seat of Pro/NC regardless the modules you get (Complete or basic) comes with a Vericut embedded license.

 

CGTech also offers another one which is much better, at a reasonable price (US$2.5K) - As PTC didn't want to transfer the R&D costs of a better interface to their customers, CGTech decided to develop and commercialize one themselves for customers that want more than the basics. We have it, and it is worth every penny.

 

HTH

 

Daniel

[Watcher]

Peon,

Don't you know that maintenance only covers the most basic of post processors?

 

Mike

 

Yes, it's true. Post-processors are one of the main sources of revenue for resselers and CAM VARs. Last Friday I heard one saying that if he could he would give seats for free just to charge for posts...

[Tyler Robertson]

Daniel - the correction and explanation was both fantastic and appreciated!