AnsweredAssumed Answered

change hole size (.dxf/drawing) depending on manufacturing process

Question asked by Lauritz Berg on Sep 14, 2020
Latest reply on Sep 15, 2020 by Ben Nemec

Like • Show 0 Likes0
Comment • 11

Maybe I am overlooking something all the time or our solidworks package does not offer this features but here is the problem:

I have the same part that I want to cut on a plasma/laser/mill with a hole size of 2" in different thicknesses.
naturally I want the hole size to be at least 2", but depending on the thickness and manufacturing process I need different hole sizes in my drawing/dxf:
the plasma needs a hole size that is bigger depending on the thickness (varies from 1/16" to 1/8" bigger depending on the thickness of the part) - the .dxf file has a hole in there that is 2.0625"
the laser needs a hole size that is usually just 0.02" bigger so the .dxf file has a hole in there that needs to be at least 2.02" in diameter

for the mill the production 'just' needs to know the correct tooling which means that the drawing shows the correct diameter of 2" with a tolerance at the bottom

Is there a possibility to automatically make those holes the correct size into the .dxf depending on the process? I.e. if I change to the custom property (laser/plasma/mill) it would put in the correct measurement into the drawing.
Or is that something that would need to be done on the nesting side (put holes onto a different layer?)? Do I need to use special features in solidworks to make this arrangement possible on the nesting side?
Is this only possible by macro?

How should I define those processes in my properties? Is there a best practice?

Recently we had to outsource many parts to different manufacturers and in the end the hole sizes were either too small or too big.

Ben Nemec Sep 15, 2020 11:41 AM

Correct Answer

Lauritz Berg wrote:

That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.

If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.

And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.

Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.

If the part is manufactured out of house, can't they make their own dxf? Send them print and maybe a model. As others have stated the dxf is for reference only as the true CNC data used is manufacturing data as opposed to design data. SOMETIMES engineering can provide the CNC data, namely dxf, and it will work out IF the stars all align. We do that internally, but do not when we purchase metal components. Save yourself the headache and let your vendors make their own dxf per their manufacturing processes, which really aren't much of your concern, then just get your dxf correct for your inhouse mfg process. Just my $0.02

See the reply in context

No one else had this question

Outcomes

Solid Air Sep 14, 2020 9:39 PM

Seems to me that it would be the manufacturer's responsibility to compensate for the process used. You print should show the size you want? At least that is how it is done where I work.

Actions

Dario Karalic @ Solid Air on Sep 15, 2020 3:59 AM

I agree with Solid Air , but as solution i would recommend to look at configurations maybe.

Actions

Lauritz Berg @ Solid Air on Sep 15, 2020 9:04 AM

That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.

If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.

And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.

Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.

Actions

Tim Taby @ Lauritz Berg on Sep 15, 2020 9:41 AM

This is why the drawing should have the nominal hole size that is required with a tolerance. Manufacturing, ether in house or outside is responsible for making it to that size no matter what process they use.

Actions

Dan Pihlaja @ Lauritz Berg on Sep 15, 2020 11:12 AM

Lauritz Berg wrote:

That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.

If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.

And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.

Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.

If your part hole CAN be bigger than is called out on the drawing and still function reliably, then maybe you should be adjusting your tolerances on the drawing to include the entire range that is acceptable. Instead of adding work by adjusting your drawing to fit the manufacturing process, just add the tolerances that you need and be done with it.

Actions

Ben Nemec @ Lauritz Berg on Sep 15, 2020 11:41 AM

Lauritz Berg wrote:

That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.

If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.

And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.

Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.

Actions

Lauritz Berg @ Ben Nemec on Sep 15, 2020 3:23 PM

If the part is manufactured out of house, can't they make their own dxf?

Usually they can or we work so close that we know what to expect when we send them a dxf. In this case we did not have the time to wait for them to do all the drawings manually thus we sent them our dxf-data to cut. I was hoping for some buried SolidWorks feature that I did not know about so if we ever encounter this problem again, we would have something ready.
Or prepare the parts correctly (in a nice best-practice manner) and have a macro take care of this problem.

Thank you all for your input though, helped me out a lot!

Actions

Ben Nemec @ Lauritz Berg on Sep 15, 2020 4:35 PM

If you're working that closely with your inhouse and purchased part suppliers so that supplying a dxf is part of your "agreement" that can create a different environment. In a past job we worked with some "Mom&Pop Shops" that were some of our best vendors so we would provide some of the manufacturing data to them with a net efficiency gain. I understand that the spectrum is wide in this respect.

I forget that some people pull dxf from the drawing, we've always generated dxfs from our model.

With all that in mind, the only thing I can think of is to use configurations. Now, I'm new to Solidworks so consider this idea with skepticism. We've been dealing with the FLAT pattern configurations recently for some other stuff so it fresh in my mind. It's my understanding that the flat view used on print is just a configuration that is automatically generated when a flat view is added to drawing, namely: DefaultSM-FLAT-PATTERN and that config is saved with the flat view turned on. You can just create more configurations for your manufacturing methods, named accordingly, with a "MoveFace - offset" feature with the D1 configured for each. Like so:

So when your "Default" config is active (green checkmark right?) then the hole size is nominal, in my part I had open is 0.38" as seen above.

Then if the DefaultSM-FLAT-PATTERN is active you have your flat pattern for print, still showing nominal hole diam.

Now when you select the FLAT_LASER the hole diameter changes:

Lastly the FLAT_Plasma config:

Now, I made a mistake here that you'll notice if you can read the measurement in screen shots. I'm not the fastest car in the derby so I made the offset values your desired diameter changes, I should have made it half, duh. I was going to fix it but I decided to share it with you all instead of taking time to go back and redo all the screen shots.

In my opinion this is a bit hack and if you're files have an infinite useful life expectancy and multiple users you'll want to make this part of your training and make sure everyone that uses Solidworks understands what's going on here so they don't botch up the configurations in future edits/revisions. One nice thing about using the offset in the flat is that if there's a change to the hole diameter down the road those configs should update just fine and still be the same offset larger than the new nominal.

Lastly, there may be hassle with getting the correct dxf for what you need. For what we have this wouldn't work at all because we have a PDM task add-in that generates the dxf would just grab the default. BUT, with some more research you can figure out how to add the configuration name into the dxf file name for the sake of quality control.

Hope that's more help than hinderance and worth the read. As I said, I'm still learning too so don't take this as the best or only way to do it. I'm sure others here could shoot this theory full of holes, but that's what we're here for is to learn from each other.

Best of luck to you.

Actions

Kevin Chandler Sep 15, 2020 10:01 AM

How should I define those processes in my properties? Is there a best practice?

Recently we had to outsource many parts to different manufacturers and in the end the hole sizes were either too small or too big.

Hello,

Unless it's an in-process drawing, part drawings only specify what's required of the final part.

How this is done is not specified on part drawings. Manufacturing personnel determine this and route the job accordingly.

When manufacturers deliver parts out of tolerance, then they are not to be paid until the contract is satisfied per the terms, which includes drawings and specifications, as these are legal documents.

This assumes your drawing actually specifies what matches your expectations and your requirements.

Review your drawing to confirm, for both size and form, the indicated information is correct toward requirements.

Then submit the part to manufacturing and let them do what they're paid to do.

Kevin

Actions

Frederick Law Sep 15, 2020 10:17 AM

Basically you need a config for each process to create dxf for each process.

Make them all different part number and file name.

You can use equation to add or minus a "process allowance" on all dimensions.

Actions

Justin Pires Sep 15, 2020 10:58 AM

Maybe you can investigate Equations using Nested IF statements: IE

(top level or user defined 1=lsr, 2=plas,3=drilled)

Process = 1 (OR 2 OR 3)

(ELSE)

1=IFF("process"=1 ,+.02,+0.0) (ELSE)

2=IFF("Process"=2, IFF("thickness"=0.75 , +0.0625 IFF("thickness"=0.25 , +0.03125))) ,+0.0

3=0

~~I know I have the syntax wrong here but its something like this. The last part is the equation that the hole dimention ~~looks to, something like beow.

Hole Dim= "1"+"2"+"3" (This would resolve as 0.02+0+0= 0.02... Process 1)

Actions

11 Replies

Solid Air Sep 14, 2020 9:39 PM
Mark Correct
Correct Answer
Seems to me that it would be the manufacturer's responsibility to compensate for the process used. You print should show the size you want? At least that is how it is done where I work.
Like • Show 6 Likes6
Actions
- Dario Karalic @ Solid Air on Sep 15, 2020 3:59 AM
  Mark Correct
  Correct Answer
  I agree with Solid Air , but as solution i would recommend to look at configurations maybe.
  Like • Show 1 Like1
  Actions
- Lauritz Berg @ Solid Air on Sep 15, 2020 9:04 AM
  Mark Correct
  Correct Answer
  That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.
  
  If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.
  
  And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.
  
  Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.
  Like • Show 0 Likes0
  Actions
  - Tim Taby @ Lauritz Berg on Sep 15, 2020 9:41 AM
    Mark Correct
    Correct Answer
    This is why the drawing should have the nominal hole size that is required with a tolerance. Manufacturing, ether in house or outside is responsible for making it to that size no matter what process they use.
    Like • Show 4 Likes4
    Actions
  - Dan Pihlaja @ Lauritz Berg on Sep 15, 2020 11:12 AM
    Mark Correct
    Correct Answer
    Lauritz Berg wrote:
    
    That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.
    
    If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.
    
    And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.
    
    Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.
    If your part hole CAN be bigger than is called out on the drawing and still function reliably, then maybe you should be adjusting your tolerances on the drawing to include the entire range that is acceptable. Instead of adding work by adjusting your drawing to fit the manufacturing process, just add the tolerances that you need and be done with it.
    Like • Show 1 Like1
    Actions
  - Ben Nemec @ Lauritz Berg on Sep 15, 2020 11:41 AM
    Unmark Correct
    Correct Answer
    Lauritz Berg wrote:
    
    That's the problem - for our plasma we adjusted the hole sizes, because the software company from the plasma software charges extra for 'True hole'-technology. Our outside of the part is up to 1/32" bigger (a part that is too small on the outside could mean that it is garbage!) on each side which led in the past to holes that were too small, so we corrected it in solidworks.
    
    If we send this out to one manufacturer who uses a laser and one who uses a plasma the .dxf has to be different for that. We send a .dxf & a drawing but I cannot tell them to double check all the hole sizes on a .dxf. That would cost too much time etc.
    
    And if we i.e. have to send out one part to a manufacturer that uses a plasma, but we need a better tolerance than what a plasma cutter can offer, they need to drill that hole according to the drawing.
    
    Right now we are using configurations but that is a real pain for the amount of parts. I was hoping there would be a better way.
    If the part is manufactured out of house, can't they make their own dxf? Send them print and maybe a model. As others have stated the dxf is for reference only as the true CNC data used is manufacturing data as opposed to design data. SOMETIMES engineering can provide the CNC data, namely dxf, and it will work out IF the stars all align. We do that internally, but do not when we purchase metal components. Save yourself the headache and let your vendors make their own dxf per their manufacturing processes, which really aren't much of your concern, then just get your dxf correct for your inhouse mfg process. Just my $0.02
    Like • Show 3 Likes3
    Actions
    - Lauritz Berg @ Ben Nemec on Sep 15, 2020 3:23 PM
      Mark Correct
      Correct Answer
      If the part is manufactured out of house, can't they make their own dxf?
      Usually they can or we work so close that we know what to expect when we send them a dxf. In this case we did not have the time to wait for them to do all the drawings manually thus we sent them our dxf-data to cut. I was hoping for some buried SolidWorks feature that I did not know about so if we ever encounter this problem again, we would have something ready.
      Or prepare the parts correctly (in a nice best-practice manner) and have a macro take care of this problem.
      
      Thank you all for your input though, helped me out a lot!
      
      Like • Show 0 Likes0
      Actions
      - Ben Nemec @ Lauritz Berg on Sep 15, 2020 4:35 PM
        Mark Correct
        Correct Answer
        If you're working that closely with your inhouse and purchased part suppliers so that supplying a dxf is part of your "agreement" that can create a different environment. In a past job we worked with some "Mom&Pop Shops" that were some of our best vendors so we would provide some of the manufacturing data to them with a net efficiency gain. I understand that the spectrum is wide in this respect.
        I forget that some people pull dxf from the drawing, we've always generated dxfs from our model.
        
        With all that in mind, the only thing I can think of is to use configurations. Now, I'm new to Solidworks so consider this idea with skepticism. We've been dealing with the FLAT pattern configurations recently for some other stuff so it fresh in my mind. It's my understanding that the flat view used on print is just a configuration that is automatically generated when a flat view is added to drawing, namely: DefaultSM-FLAT-PATTERN and that config is saved with the flat view turned on. You can just create more configurations for your manufacturing methods, named accordingly, with a "MoveFace - offset" feature with the D1 configured for each. Like so:
        
        So when your "Default" config is active (green checkmark right?) then the hole size is nominal, in my part I had open is 0.38" as seen above.
        
        Then if the DefaultSM-FLAT-PATTERN is active you have your flat pattern for print, still showing nominal hole diam.
        
        Now when you select the FLAT_LASER the hole diameter changes:
        
        Lastly the FLAT_Plasma config:
        
        Now, I made a mistake here that you'll notice if you can read the measurement in screen shots. I'm not the fastest car in the derby so I made the offset values your desired diameter changes, I should have made it half, duh. I was going to fix it but I decided to share it with you all instead of taking time to go back and redo all the screen shots.
        
        In my opinion this is a bit hack and if you're files have an infinite useful life expectancy and multiple users you'll want to make this part of your training and make sure everyone that uses Solidworks understands what's going on here so they don't botch up the configurations in future edits/revisions. One nice thing about using the offset in the flat is that if there's a change to the hole diameter down the road those configs should update just fine and still be the same offset larger than the new nominal.
        
        Lastly, there may be hassle with getting the correct dxf for what you need. For what we have this wouldn't work at all because we have a PDM task add-in that generates the dxf would just grab the default. BUT, with some more research you can figure out how to add the configuration name into the dxf file name for the sake of quality control.
        
        Hope that's more help than hinderance and worth the read. As I said, I'm still learning too so don't take this as the best or only way to do it. I'm sure others here could shoot this theory full of holes, but that's what we're here for is to learn from each other.
        
        Best of luck to you.
        Like • Show 1 Like1
        Actions
Kevin Chandler Sep 15, 2020 10:01 AM
Mark Correct
Correct Answer
How should I define those processes in my properties? Is there a best practice?

Recently we had to outsource many parts to different manufacturers and in the end the hole sizes were either too small or too big.
Hello,

Unless it's an in-process drawing, part drawings only specify what's required of the final part.
How this is done is not specified on part drawings. Manufacturing personnel determine this and route the job accordingly.

When manufacturers deliver parts out of tolerance, then they are not to be paid until the contract is satisfied per the terms, which includes drawings and specifications, as these are legal documents.

This assumes your drawing actually specifies what matches your expectations and your requirements.
Review your drawing to confirm, for both size and form, the indicated information is correct toward requirements.

Then submit the part to manufacturing and let them do what they're paid to do.

Kevin
Like • Show 4 Likes4
Actions
Frederick Law Sep 15, 2020 10:17 AM
Mark Correct
Correct Answer
Basically you need a config for each process to create dxf for each process.
Make them all different part number and file name.
You can use equation to add or minus a "process allowance" on all dimensions.
Like • Show 1 Like1
Actions
Justin Pires Sep 15, 2020 10:58 AM
Mark Correct
Correct Answer
Maybe you can investigate Equations using Nested IF statements: IE
(top level or user defined 1=lsr, 2=plas,3=drilled)

Process = 1 (OR 2 OR 3)
(ELSE)
1=IFF("process"=1 ,+.02,+0.0) (ELSE)
2=IFF("Process"=2, IFF("thickness"=0.75 , +0.0625 IFF("thickness"=0.25 , +0.03125))) ,+0.0
3=0

~~I know I have the syntax wrong here but its something like this. The last part is the equation that the hole dimention ~~looks to, something like beow.

Hole Dim= "1"+"2"+"3" (This would resolve as 0.02+0+0= 0.02... Process 1)
Like • Show 1 Like1
Actions

change hole size (.dxf/drawing) depending on manufacturing process

Outcomes

Related Content

Recommended Content