Need Help!- Profile Operation??

[pinguS]

Hi

I think this is the right operation, but I'm getting stuck right at the beginning. I know this must be simple but if I just have a solid piece of material, say 6" square or round. I want to be able to just profile a shape down.

More explaination:
The thing Im trying to make looks a pair of bonoculars, sort of, i.e. a 50mm diamter circle in the middle 80mm depth. Connected to this are 2 stems either side half way down, but these are only 20mm, square. And on the ends of these are 2 circles 30mm diameter also only 20mm depth (so these are in located exactly 40mm down centre to centre)

When I select profile, if I need to just mill the external shape down, I imagine you have to use "Curve and Auto-constant Z" to define the profile, but where the stems connect to the main circle, being half way down, it doesn't have any lines to select, only a face, which then alarms "Chain must be continuous"

I have a 80mm depth by 6" billet clamped down (6" round). All I'm need to do is profile the outer shape out, the rest I can hopefully manage to set up in Solidcam. The part is solidworks.

So was wondering how the heck do I mill a shape out, just external shape if I can't select lines?

Does this make any sense at all?? I have attached a picture of what I'm making

[Brakeman Bob]

There are various ways of tackling this. One is to go to the feature tree in SW, right click on CAM part and select "Edit Part". Then select the top face of the part, right click and select "Insert Sketch". Once in the sketch select the edges you want to form the profile and convert the entities to sketch lines. Stop editing the sketch, go to you SolidCAM job and define the profile from the sketch you've just created. Voilá.

Another way is to open up the CAM part for editing, select (or create) the plane which bisects the part at a place where the profile is as you want it and ceate a sketch. Then via sketch tools selrct "Intersection Curve" and pick the faces of the profile. Then define the geometry as before.

The CAM part is a very powerful tool in defining geometry and opens up all the usability of SolidWorks for controlling the tool path. For example, setting up a work area or constraint boundary, offsetting a face and filling it to act as a mask in 3D machining. I'd be lost without it.

[pinguS]

....The CAM part is a very powerful tool in defining geometry and opens up all the usability of SolidWorks for controlling the tool path. For example, setting up a work area or constraint boundary, offsetting a face and filling it to act as a mask in 3D machining. I'd be lost without it. ....

Can you explain more on this, or when you say open up the cam part, do you mean actually open a file in solidworks which has been created in solidcam??

Brakeman, I really hope Solidcam have given you excessive shares in their business, assuming you are not linked to them, as I don't actually know where they would be without you.....

[pinguS]

Ok that worked, using a profile line created in solidworks, which has led me to another problem I though would be easily solved, but I'm struggling....

If you look at the 2 circle lugs to either side of the big circle, I thought I obviously need to use a face mill operation to bring them down to the right height (currently still has stock material to machine off), but using this it cuts straight through the big circle, not around it. I have even tried by separating each face when defining the contours.

Should I be creating seperate operations for each side circle, instead of trying in one operation? Or am I just using the wrong operation.

I have tried profile again, but it just doesnm't calculate anything (nothing showing in the simulation...)

hmmmmmm

[pinguS]

Ok another thing I have just tried, or tried to do was change the direction of the face operation, but I can't seem to get it to go back and forth in Y axis direction, it only seems to go in X axis back and forth...

..........Ok worked this out, this is the angle setting in data setting for Hatch on face operation.... but still struggling to machine down the side circles

[Brakeman Bob]

Originally Posted by pinguS ....The CAM part is a very powerful tool in defining geometry.....Can you explain more on this, or when you say open up the cam part, do you mean actually open a file in solidworks which has been created in solidcam?? Brakeman, I really hope Solidcam have given you excessive shares in their business, assuming you are not linked to them, as I don't actually know where they would be without you.....

When you are working in SolidCAM, the Solidworks window is showing and assembly - your part is named "Widget.SLDASM" - and looking in the SolidWorks Feature Tree shows at least two parts

"DesignPart" - this is the clone of the part you are programming code for. SolidCAM creates the clone so that nothing untoward happens to your original and for speed purposes. This clone is associated with the original and if the designer changes the original model SolidCAM will rpompt you to decide if you want to update tour "DesignPart". Do not mess with the DesignPart as it can have odd outcomes if the original is changed.

The other part is the "CAM Part". This is an empty part created by SolidCAM for you to do your stuff in (if you put sketches etc. in at the assembly level it don't half slow down processing if you have a big part and lots of sketches). This part is associated with the "DesignPart" and therefore if say you create a sketch using entities in the DesignPart which change, your sketch will change. You can do anything you like in the "CAM Part" - it is what it is there for.

Of course there is nothing stopping you from adding to the assembly - I have all our fixtures modelled, so I add them in order to do collision checking. I also add the billet or forging from which the part is machined and then use this model to define my stock.

I don't have shares in SolidCAM - I am just a (relatively) happy user who like to pass his knowledge on. I think sometimes that SolidCAM get a little fed up with me as I do seem to find bugs that no-one else reports, but I put that down to the complexity of our parts and my determination to stretch the software.

[Brakeman Bob]

Originally Posted by pinguS Ok another thing I have just tried, or tried to do was change the direction of the face operation, but I can't seem to get it to go back and forth in Y axis direction, it only seems to go in X axis back and forth... ..........Ok worked this out, this is the angle setting in data setting for Hatch on face operation.... but still struggling to machine down the side circles

If you have defined your billet you could use the outer edges for a profile job to machine the side circles. Go to the Technology tab and click on "Geometry" to extend or offset the lines. Alternatively sketch a horseshoe shap in CAM Part and use that in a Profile job. The cutter path doesn't have to be linked directly to the part geometry.

[pinguS]

I didn't actually think of that (horse shoe)

I was assuming use would just select the areas to machine and solidcam would pick up on the fact is was going to cut away at an undefined area of the part (the big circle), which would then change the final part when side circles are machined.

Can machining boundaries not be defined, i.e. tell solidcam it cannot cross the big circle profile when calculating machining of the small circles. Either way, i'm going to go with horse shoe style and see what I get...

[Brakeman Bob]

No CAM system I'm aware of is that smart. Delcam's PowerMIll comes close but it is amied more at the Mould & Die sector (at least it used to be).

[dengo]

If you have HSM you can also use the combined boundary option which will allow you to play around with the interaction of previously used boundaries to produce new ones.
But the best advice with SC is KISS......

[Brakeman Bob]

Originally Posted by dengo If you have HSM you can also use the combined boundary option which will allow you to play around with the interaction of previously used boundaries to produce new ones. But the best advice with SC is KISS......

I've seen that combined boundary option and I believe that you can also do boolean operations with boundaries. Never have cause to use it yet but I am intrigued.

[pinguS]

What part of solidcam are you guys talking about, how do I check If I have the HSM options as this is not my company, and the owners are lets say not so clued up...

I would like to know more on this boundary option...