part instances to drawing files

[cadcamguy]

It's probably happened before to someone else.
But I have the need to make drawings of all instance of a generic part.
Granted I could have a repeat region table to show all flavors but I need to eventually get 1:1 dxf files to export for machining purposes.
I create a drawing off the generic... dim it <though not really needed... does clarify> save that to model name

Now I replace model with an instance, great it's dimmed also, now I save under instance name and so on and so forth thru all the different instances... getting to be a tedious chore and I am looking at this again with another model.

This can't be the right method, there has to be a better way... rehashing a trail file which is the only suggestion I have found on the web ... isn't all that great. since you have to type in the names also.

I can pro_batch the drw to dxf, no problem, but not until get the drw's

Any thought out there? Or is this a taboo subject

 

[Tofflemire]

Hi Cadcamguy,

What I do for this... Dimension your first part, and then add your instance and a view of it, you only have to dim what is different or added to this from the main view. Lets say you have added a hole to your instance and that is the only thing that is different then in that view the only dimensions required are to locate that hole. If you have many different instances than you just add any dim that is not show yet to the drawing....


Tofflemire

 

[cadcamguy]

Hi Tofflemire,

There are no additional details, they are are basically the same except for sizes and locations of holes etc.Which I have set up in the table.

I wondering if there is a way to get around having to replace the model and then save it again with the new name.

The replace model box defaults to generic, so I have to scroll down find the next instance and click it, I can't mapkey the instance box to go to the next one, it always starts at generic, the top. ... arrow down or page down none of those keys respond while I am in mapkey record.

Also I can't use the &model_name drawing parameter for the new drawing name.. it does like the "&" in the name. Maybe it could be back written to a string parameter, but I really think it's not going to work as it will take it as a literal value regardless.

It's turning into a mouse and keyboarding ordeal :-(

Does that make more sense?
Bill

 

[Tofflemire]

Hi Cadcamguy,

We put like parts on the same drawing, but with variations like -01, -02... We would not create a new drawing but just add another view on the sheet.

Tofflemire

 

[cadcamguy]

Tofflemire,
Okay I see what you are saying......add model to drawing then use it to add view.

It's looking like I have to redim and I am not getting my &model_name note passed it with it

I can add that too but it's looking like it goes with what the last one is

I still have to scroll thru the instance box to select

I was hoping for a way to automate this so I can run the mapkay and it output all the instances automagically.

I don't want too much do I ;-)

 

[Tofflemire]

Hi Cadcamguy,

I am confused to why you have to dimension so many different steps. You just have to dimension the final part you want. Are these all the same part number? You could also just add sheets for each variation. I still think I am missing what your goal is.

Tofflemire

 

[cadcamguy]

Tofflemire,

Well the goal is to supply the machine shop with all instances of the generic part in dxf format so they can just drop in the new art and pick the changing hole locations,pockets and profiles.
They can keep all their existing tool setup and cut parameters, just update to geometry. It's mastercam, not pro/man, so I can't load the generic and change models.

But I think with the method of adding the model<instance> to the drawing on a new sheet each time would be a good deal easier, I'd still have to pick in the instance box but I wouldn't have to save under a new name each time.

I bet if I create a format with the &model_name in a table
it will come along for the ride then.

I'm am surprised that when I bring in a new instance it doesn't bring in the dims and note I created on the generic... but really a minor detail as long as they know which is which.

This helps as I have 400+ to go through... Make sense?
Guess I better found out how well Mcam accepts different sheets before I get too far..

Thanks Tofflemire !!
Bill..Time for a test run

 

[JB36]

Hello,

To automate your process of generating your drawings for all instances, you should have a look to the weblink capabilities. In Wildfire it is quite easy to developp small scripts using javascript, and to run them directly in the embeded internet explorer of Wildfire.

You have to be familiar with HTML, and Javascript programming techniques.
Look in <install point>/weblink you will find all documentation and some examples.

Hope this helps.

 

[cadcamguy]

What I did come up with is using WORD's VBA to read the list of instances and generate a mapkey with the different name and address's so to speak, of open and save as values of the single mapkey.

Saving that to one big mapkey, minding the 2048 length restriction of a single mapkey. Chaining them when necessary.

Then I load the new config.pro VBA makes, change work dir to a empty folder and output the drawings while I get a cup of coffee. Takes about 10 mins. to output 600 dimensioned drawings. Based on the generic's dims.

It has worked flawless so far. The only odd thing is when it's done. It shows the generic model referenced in the model tree on xxx instance, but if you close drawing out and erase not displayed it's all in sync. Inst. Model to Inst.Drawing name.

Now I can Pro_Batch the drawings to DXF getting a second and third cup of coffee.

I'm seeing this as a pretty wide open type of alternative to passing parameters around. Because you can tell Word which macro to run on startup.

The Java/Html way sounds good too. But I am on R2001, someday WF, but it should work in WF also. Between outputing the tree info,inf files,instance files there is a good deal of infromation to be grabbed outside of Pro.