Hole Recognition/Machining Process tables, anyone use them?

[glovebox20]

Hello

I was wondering if anyone uses the Machining Process Table/ Hole Recognition to program there parts.

I was hoping some could point me in the right dircection useing this feature being this feature is not well documented.

Thanks

Glovebox20

[Brakeman Bob]

I use Machine Processes and I have looked into Hole Recognition.

I like Machine Processes. They take a little time to set up but if you have standard features on your parts Machine Processes are an excellent way of ensuring consistency. My only gripe with MP's is there is no provision to use string variables - for example to insert to insert the Geometry name into the Job Description.

Hole recognition is very powerful under the right circumstances but it I don't use it because it doesn't cope (or I can't get it to cope) well in two areas. These are firstly holes which have standard features at some point along the holes length but are in non-standard positions to the top of the hole (for example a threaded & counterbored hole on an oblique or curved surface). The second area where I have problems is making the automation recognise updated stock. For example, I machine parts out of big rectangular billets and sometimes I need to machine some of the billet away to provide a flat on which to start my hole but this flat is (say) 20mm above the final geometry of the part. Hole recognithin eithere sees the initial raw stock or the finished part, not the updated stock model.

Have you investigated the Templates facility? I cannot get these to work well for me at all as they don't have the variables like in Machine Processes which is a shame because MP's don't work with HSM or 5X and Templates do.

[glovebox20]

I have been playing around with the MP tables. I havn't gotten to far with them yet, but do I do think it would be a better alterntive to Process Templates for drilling holes/programing pockets once I figure it out. I bigest thing I'm working with is trying to figure out the best way to make use of my standard Tool table, and creating tools that aren't in the table while appling the correct Speed/Feed.

I'm using InvenrCam2011 and found plenty of error's in the Standard MP tables, witch isn't making it any easier to learn. Templates are quick and easy to create, but I don't like how you have to go back and apply the Geom. to every operation and check the levels after inserting.

I opened up the Hole Rec. but never got any where with it. It's seems a little over my head without anyone showing me how to get started.

I though I start this thread to see how many people use these features and how they are applling them to there appicaltion. I called my local soildcam Rep. to ask him about the MP tables, and I knew more about it than he did

glovebox20

[Brakeman Bob]

I found that the best way to create a Machine Process was to create the sequence of tools / jobs in 'ordinary' SolidCAM then select them as a group, right click and go "Create Operations Group". This gathers all the selected jobs together under one heading. Then with this group selected right click once again, go "operations group" and now click the option to "Make Machine Process from this Group". The explode the group and go to the MP table where you find your latest MP added. But it ain't over yet - you need to edit the jobs within the group to reset the clearance level and safety level to CAM system variables. This also gives you the chance to create and define any user variable you wish like "DATUM" or "DEPTH". One really useful thing to do is create a user variable for tool_number and use this in the jobs to give you the chance to designate tool at the time of use. If, like me you use a standard tool library and wish to call a fixed tool within that library you can right click the tool in the MP job tree, go to select tool and by right clicking once again you can select an option to just designate a tool number and the MP will just pict that tool from the tool library. However, it a then a good idea to go to the tool tab in each job check the box to use the default tool data from the tool library as this will then reflect the data you are currently using and not the data set when you created the MP.

Machine Processes save me a lot of time and make my programming more consistent in some key areas, namely drilled & threaded holes with 4 or 5 different diameters and depths in precise relationship to each other. They are also good for simple simple sequences such as a PREP program consisting of facing off a billet, drilling & tapping half a dozen holes and drilling & reaming a couple more - I can create that program from scratch in less than 2 minutes.

The Hole Recognition package promises much to the person who invests the time in getting deep & dirty into the guts of it and understanding the logic. I have spent some time with it and, yes, it has it's uses particularly in rapidly creating MAC positions for angled holes (I have gone up to 32 MAC positions in one part before now). But I am too busy just at the minute to invest the time to study, test and develop it for my needs and I think that goes for a lot of people.

I do worry that MP's have become a 'forgotten' technology and support for it will quietly drop away, but if they start to include variables in Templates and promote those as the replacement for MP's then I for one will be willing to move over.

[glovebox20]

Thanks for the Tips Brakeman.

I agree, if they could combine the things I like about Templates and MP tables together, that would be pretty sweet.

For Tools not in your machine tool table, how would you include these in the MP tables?

Would you create all the tools and put them in one table, or use seprate tables to make finding them easier?

I was thinking about creating a MP table using varables based off the tool dia. to create tools (length, tip angle, # of flutes,ect.) not in the Tool table. The thing I don't like about this is that you would have to creat a MP based off your standard tools, and another tools not in the Tool table.

glovebox20

[Brakeman Bob]

The tools must be defined somewhere, either in your default tool library that is loaded when a new CAM part is created or in the part tool library or in the MP tool library that is defined when you create the MP. I don't think you can define a tool when the MP is executed.

There are ways of changing a tool during the execution of the MP by defining the tool number as a variable that is set when the MP is executed but the tools would still have to be defined in the part tool table or the MP tool table.

I use a system of standard tool libraries, one for 5 axis machines, one for the horizontals, one for the verticals etc. that are loaded by default according to which post processor I am using. These libraries are accurate and well maintained. My MP's only call tools which are present in those libraries (it follows that I have different MP files for different machines too). If I need to use a tool not currently in the library, I define the tool first in the 'master' library and then import it into the part. This is tedious, I know, but the discipline is crucial to the way we work here. As I said in my first post, I use MP's to provide consistency when machining standard features, not as a way of automating my general machining, so my needs are a bit specialied I suppose.

One area I hoping to get into, unrelated to MP's but critical to tool libraries, is the defining of work material, tool material and different speed & feeds. I have looked at this a couple of times and given up in the end. I currently have tool libraries for different materials eg 5 axis Aluminium, 5 Axis Steel etc.

One day I'll crack it....

[glovebox20]

Right now I have my tool libraries with the work material (Steel and Alum right now being that is all we machine) and I'm not completely sold on the idea. It works fine as long are your tools are define before you select your work material in the cam-part definition. If you import tools from another libary, you have to manualy select the work material type for that tool when importing, or redefine your work material in the cam-part definition to get the speed and feed to update. It seems to me it might be just as easy to have your to libraries set up with just one material type, and have a libray for each work material.

Thanks for your tips Brakeman

glovebox20

[Brakeman Bob]

Thanks for your observations on work materials. I think I will continue with my method of a separate library for each material group. This can make for hard work, especially on the mill-turn machines where we handle a lot of different materials - Aluminium, Steel, Alloy Steel, Titanium, Austenic Stainless, Martensitic Stainless, Cast Iron and MMC and the tool geometries are the same. What I do is When I add a new tool to (say) the TI library I straight away copy it in to all the others and modify the speeds & feeds otherwise I forget what I have put in each library. Tedious, it's true, but I can't rely on my memory like I used to.